はじめに
境界条件タイプリストの表示について。
使用バージョン
OpenFOAM 4.x (blueCFD)
境界条件タイプリスト
OpenFOAM の境界条件タイプの説明のリストが必要な場合がある。各タイプの説明はソースコードのコメントの Discription に書かれているので、それを並べられればよい。以下のようなスクリプトでリストが得られる (抜けや余分なものがあるかも)。標準ソルバー独自のものもあるので、それも表示している。説明がないものもある。
show_patch_types
#!/bin/sh
COUNT=0
for DIR in $FOAM_SRC $FOAM_SOLVERS ; do
cd $DIR
for PATCH_PATH in `find | sort -f | grep FvPatch | grep -v lnInclude | grep "Field\.H$" | xargs -I {} dirname {} | sed -e "s%^./%%" | uniq` ; do
echo $PATCH_PATH
echo
cat $PATCH_PATH/*Field.H | awk '
/\\\*/ {exit}
/SourceFiles/ {exit}
a == 1 {print}
/Description/ {a = 1}
'
echo
echo
COUNT=`expr $COUNT + 1`
done
done
echo Total $COUNT
実行結果
finiteVolume/cfdTools/general/SRF/derivedFvPatchFields/SRFFreestreamVelocityFvPatchVectorField
Freestream velocity condition to be used in conjunction with the single
rotating frame (SRF) model (see: SRFModel class)
Given the free stream velocity in the absolute frame, the condition
applies the appropriate rotation transformation in time and space to
determine the local velocity using:
\f[
U_p = cos(\theta)*U_{Inf} + sin(theta) (n^UInf) - U_{p,srf}
\f]
where
\vartable
U_p = patch velocity [m/s]
U_{Inf} = free stream velocity in the absolute frame [m/s]
theta = swept angle [rad]
n = axis direction of the SRF
U_{p,srf} = SRF velocity of the patch
\endvartable
Usage
\table
Property | Description | Required | Default value
UInf | freestream velocity | yes |
relative | UInf relative to the SRF? | no |
\endtable
Example of the boundary condition specification:
\verbatim
{
type SRFFreestreamVelocity;
UInf uniform (0 0 0);
relative no;
value uniform (0 0 0); // initial value
}
\endverbatim
See also
Foam::freestreamFvPatchField
Foam::SRFVelocityFvPatchVectorField
finiteVolume/cfdTools/general/SRF/derivedFvPatchFields/SRFVelocityFvPatchVectorField
Velocity condition to be used in conjunction with the single
rotating frame (SRF) model (see: SRFModel class)
Given the free stream velocity in the absolute frame, the condition
applies the appropriate rotation transformation in time and space to
determine the local velocity.
The optional \c relative flag switches the behaviour of the patch
such that:
- relative = yes: inlet velocity applied 'as is':
\f[
U_p = U_{in}
\f]
- relative = no : SRF velocity is subtracted from the inlet velocity:
\f[
U_p = U_{in} - U_{p,srf}
\f]
where
\vartable
U_p = patch velocity [m/s]
U_{in} = user-specified inlet velocity
U_{p,srf} = SRF velocity
\endvartable
Usage
\table
Property | Description | Required | Default value
inletValue | inlet velocity | yes |
relative | inletValue relative motion to the SRF? | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type SRFVelocity;
inletValue uniform (0 0 0);
relative yes;
value uniform (0 0 0); // initial value
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/cfdTools/general/SRF/derivedFvPatchFields/SRFWallVelocityFvPatchVectorField
Wall-velocity condition to be used in conjunction with the single rotating
frame (SRF) model (see: FOAM::SRFModel)
The condition applies the appropriate rotation transformation in time and
space to determine the local SRF velocity of the wall.
\f[
U_p = - U_{p,srf}
\f]
where
\vartable
U_p = patch velocity [m/s]
U_{p,srf} = SRF velocity
\endvartable
The normal component of \f$ U_p \f$ is removed to ensure 0 wall-flux even
if the wall patch faces are irregular.
Usage
Example of the boundary condition specification:
\verbatim
{
type SRFWallVelocity;
value uniform (0 0 0); // Initial value
}
\endverbatim
See also
Foam::SRFModel
Foam::SRFVelocityFvPatchVectorField
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/basic/basicSymmetry
A symmetry patch
finiteVolume/fields/fvPatchFields/basic/calculated
This boundary condition is not designed to be evaluated; it is assmued
that the value is assigned via field assignment, and not via a call to
e.g. \c updateCoeffs or \c evaluate.
Usage
Example of the boundary condition specification:
\verbatim
{
type calculated;
value uniform (0 0 0); // Required value entry
}
\endverbatim
finiteVolume/fields/fvPatchFields/basic/coupled
Abstract base class for coupled patches.
finiteVolume/fields/fvPatchFields/basic/directionMixed
Base class for direction-mixed boundary conditions.
finiteVolume/fields/fvPatchFields/basic/extrapolatedCalculated
This boundary condition applies a zero-gradient condition from the patch
internal field onto the patch faces when \c evaluated but may also be
assigned. \c snGrad returns the patch gradient evaluated from the current
internal and patch field values rather than returning zero.
Usage
Example of the boundary condition specification:
\verbatim
{
type extrapolatedCalculated;
}
\endverbatim
finiteVolume/fields/fvPatchFields/basic/fixedGradient
This boundary condition supplies a fixed gradient condition, such that
the patch values are calculated using:
\f[
x_p = x_c + \frac{\nabla(x)}{\Delta}
\f]
where
\vartable
x_p | patch values
x_c | internal field values
\nabla(x)| gradient (user-specified)
\Delta | inverse distance from patch face centre to cell centre
\endvartable
Usage
\table
Property | Description | Required | Default value
gradient | gradient | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedGradient;
gradient uniform 0;
}
\endverbatim
finiteVolume/fields/fvPatchFields/basic/fixedValue
This boundary condition supplies a fixed value constraint, and is the base
class for a number of other boundary conditions.
Usage
\table
Property | Description | Required | Default value
value | Patch face values | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedValue;
value uniform 0; // Example for scalar field usage
}
\endverbatim
finiteVolume/fields/fvPatchFields/basic/mixed
This boundary condition provides a base class for 'mixed' type boundary
conditions, i.e. conditions that mix fixed value and patch-normal gradient
conditions.
The respective contributions from each is determined by a weight field:
\f[
x_p = w x_p + (1-w) \left(x_c + \frac{\nabla_\perp x}{\Delta}\right)
\f]
where
\vartable
x_p | patch values
x_c | patch internal cell values
w | weight field
\Delta| inverse distance from face centre to internal cell centre
w | weighting (0-1)
\endvartable
Usage
\table
Property | Description | Required | Default value
valueFraction | weight field | yes |
refValue | fixed value | yes |
refGrad | patch normal gradient | yes |
\endtable
Note
This condition is not usually applied directly; instead, use a derived
mixed condition such as \c inletOutlet
See also
Foam::inletOutletFvPatchField
finiteVolume/fields/fvPatchFields/basic/sliced
Specialization of fvPatchField which creates the underlying
fvPatchField as a slice of the given complete field.
The destructor is wrapped to avoid deallocation of the storage of the
complete fields when this is destroyed.
Should only used as a template argument for SlicedGeometricField.
See also
Foam::fvPatchField
finiteVolume/fields/fvPatchFields/basic/transform
Foam::transformFvPatchField
finiteVolume/fields/fvPatchFields/basic/zeroGradient
This boundary condition applies a zero-gradient condition from the patch
internal field onto the patch faces.
Usage
Example of the boundary condition specification:
\verbatim
{
type zeroGradient;
}
\endverbatim
finiteVolume/fields/fvPatchFields/constraint/cyclic
This boundary condition enforces a cyclic condition between a pair of
boundaries.
Usage
Example of the boundary condition specification:
\verbatim
{
type cyclic;
}
\endverbatim
Note
The patches must be topologically similar, i.e. if the owner patch is
transformed to the neighbour patch, the patches should be identical (or
very similar).
finiteVolume/fields/fvPatchFields/constraint/cyclicACMI
This boundary condition enforces a cyclic condition between a pair of
boundaries, whereby communication between the patches is performed using
an arbitrarily coupled mesh interface (ACMI) interpolation.
Usage
Example of the boundary condition specification:
\verbatim
{
type cyclicACMI;
}
\endverbatim
See also
Foam::AMIInterpolation
finiteVolume/fields/fvPatchFields/constraint/cyclicAMI
This boundary condition enforces a cyclic condition between a pair of
boundaries, whereby communication between the patches is performed using
an arbitrary mesh interface (AMI) interpolation.
Usage
Example of the boundary condition specification:
\verbatim
{
type cyclicAMI;
}
\endverbatim
Note
The outer boundary of the patch pairs must be similar, i.e. if the owner
patch is transformed to the neighbour patch, the outer perimiter of each
patch should be identical (or very similar).
See also
Foam::AMIInterpolation
finiteVolume/fields/fvPatchFields/constraint/cyclicSlip
This boundary condition is a light wrapper around the cyclicFvPatchField
condition, providing no new functionality.
Usage
Example of the boundary condition specification:
\verbatim
{
type cyclicSlip;
}
\endverbatim
See also
Foam::cyclicFvPatchField
finiteVolume/fields/fvPatchFields/constraint/empty
This boundary condition provides an 'empty' condition for reduced
dimensions cases, i.e. 1- and 2-D geometries. Apply this condition to
patches whose normal is aligned to geometric directions that do not
constitue solution directions.
Usage
Example of the boundary condition specification:
\verbatim
{
type empty;
}
\endverbatim
finiteVolume/fields/fvPatchFields/constraint/jumpCyclic
This boundary condition provides a base class for coupled-cyclic
conditions with a specified 'jump' (or offset) between the values
See also
Foam::cyclicFvPatchField
finiteVolume/fields/fvPatchFields/constraint/jumpCyclicAMI
This boundary condition provides a base class that enforces a cyclic
condition with a specified 'jump' (or offset) between a pair of boundaries,
whereby communication between the patches is performed using an arbitrary
mesh interface (AMI) interpolation.
See also
Foam::cyclicAMIFvPatchField
finiteVolume/fields/fvPatchFields/constraint/nonuniformTransformCyclic
This boundary condition enforces a cyclic condition between a pair of
boundaries, incorporating a non-uniform transformation.
finiteVolume/fields/fvPatchFields/constraint/processor
This boundary condition enables processor communication across patches.
Usage
Example of the boundary condition specification:
\verbatim
{
type processor;
}
\endverbatim
finiteVolume/fields/fvPatchFields/constraint/processorCyclic
This boundary condition enables processor communication across cyclic
patches.
Usage
Example of the boundary condition specification:
\verbatim
{
type processor;
}
\endverbatim
See also
Foam::processorFvPatchField
finiteVolume/fields/fvPatchFields/constraint/symmetry
This boundary condition enforces a symmetry constraint
Usage
Example of the boundary condition specification:
\verbatim
{
type symmetry;
}
\endverbatim
finiteVolume/fields/fvPatchFields/constraint/symmetryPlane
This boundary condition enforces a symmetryPlane constraint
Usage
Example of the boundary condition specification:
\verbatim
{
type symmetryPlane;
}
\endverbatim
finiteVolume/fields/fvPatchFields/constraint/wedge
This boundary condition is similar to the cyclic condition, except that
it is applied to 2-D geometries.
Usage
Example of the boundary condition specification:
\verbatim
{
type wedge;
}
\endverbatim
See also
Foam::cyclicFvPatchField
finiteVolume/fields/fvPatchFields/derived/activeBaffleVelocity
This velocity boundary condition simulates the opening of a baffle due
to local flow conditions, by merging the behaviours of wall and cyclic
conditions. The baffle joins two mesh regions, where the open fraction
determines the interpolation weights applied to each cyclic- and
neighbour-patch contribution.
We determine whether the baffle is opening or closing from the sign of
the net force across the baffle, from which the baffle open fraction is
updated using:
\f[
x = x_{old} + sign(F_{net})\frac{dt}{DT}
\f]
where
\vartable
x | baffle open fraction [0-1]
x_{old} | baffle open fraction on previous evaluation
dt | simulation time step
DT | time taken to open the baffle
F_{net} | net force across the baffle
\endvartable
The open fraction is then applied to scale the patch areas.
Usage
\table
Property | Description | Required | Default value
p | pressure field name | no | p
cyclicPatch | cylclic patch name | yes |
orientation | 1 or -1 used to switch flow direction | yes|
openFraction | current opatch open fraction [0-1]| yes |
openingTime | time taken to open the baffle | yes |
maxOpenFractionDelta | max open fraction change per timestep | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type activeBaffleVelocity;
p p;
cyclicPatch cyclic1;
orientation 1;
openFraction 0.2;
openingTime 5.0;
maxOpenFractionDelta 0.1;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
Foam::cyclicFvPatchField
finiteVolume/fields/fvPatchFields/derived/activePressureForceBaffleVelocity
This boundary condition is applied to the flow velocity, to simulate the
opening or closure of a baffle due to local pressure or force changes,
by merging the behaviours of wall and cyclic conditions.
The baffle joins two mesh regions, where the open fraction determines
the interpolation weights applied to each cyclic- and neighbour-patch
contribution. This means that this is boundary condition is meant to be
used in an extra wall beyond an existing cyclic patch pair. See PDRMesh
for more details.
Once the threshold is crossed, this condition activated and continues to
open or close at a fixed rate using
\f[
x = x_{old} + s \times \frac{dt}{DT}
\f]
where
\vartable
x | baffle open fraction [0-1]
x_{old} | baffle open fraction on previous evaluation
s | sign for orientation: 1 to open or -1 to close
dt | simulation time step
DT | time taken to open the baffle
\endvartable
The open fraction is then applied to scale the patch areas.
Usage
\table
Property | Description | Required | Default value
p | pressure field name | no | p
cyclicPatch | cyclic patch name | yes |
orientation | 1 to open or -1 to close | yes|
openFraction | current open fraction [0-1] | yes |
openingTime | time taken to open or close the baffle | yes |
maxOpenFractionDelta | max fraction change per timestep | yes |
minThresholdValue | minimum absolute pressure or
force difference for activation | yes |
forceBased | force (true) or pressure-based (false) activation | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type activePressureForceBaffleVelocity;
p p;
cyclicPatch cyclic1;
orientation 1;
openFraction 0.2;
openingTime 5.0;
maxOpenFractionDelta 0.1;
minThresholdValue 0.01;
forceBased false;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/advective
This boundary condition provides an advective outflow condition, based on
solving DDt(psi, U) = 0 at the boundary.
The standard (Euler, backward, CrankNicolson, localEuler) time schemes are
supported. Additionally an optional mechanism to relax the value at
the boundary to a specified far-field value is provided which is
switched on by specifying the relaxation length-scale \c lInf and the
far-field value \c fieldInf.
The flow/wave speed at the outlet is provided by the virtual function
advectionSpeed() the default implementation of which requires the name of
the flux field \c (phi) and optionally the density \c (rho) if the
mass-flux rather than the volumetric-flux is given.
The flow/wave speed at the outlet can be changed by deriving a specialised
BC from this class and over-riding advectionSpeed() e.g. in
waveTransmissiveFvPatchField the advectionSpeed() calculates and returns
the flow-speed plus the acoustic wave speed creating an acoustic wave
transmissive boundary condition.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
fieldInf | value of field beyond patch | no |
lInf | distance beyond patch for \c fieldInf | no |
\endtable
Example of the boundary condition specification:
\verbatim
{
type advective;
phi phi;
}
\endverbatim
Note
If \c lInf is specified, \c fieldInf will be required; \c rho is only
required in the case of a mass-based flux.
finiteVolume/fields/fvPatchFields/derived/codedFixedValue
Constructs on-the-fly a new boundary condition (derived from
fixedValueFvPatchField) which is then used to evaluate.
Usage
Example:
\verbatim
{
type codedFixedValue;
value uniform 0;
name rampedFixedValue; // name of generated BC
code
#{
operator==(min(10, 0.1*this->db().time().value()));
#};
//codeInclude
//#{
// #include "fvCFD.H"
//#};
//codeOptions
//#{
// -I$(LIB_SRC)/finiteVolume/lnInclude
//#};
}
\endverbatim
A special form is if the 'code' section is not supplied. In this case
the code is read from a (runTimeModifiable!) dictionary system/codeDict
which would have a corresponding entry:
\verbatim
{
code
#{
operator==(min(10, 0.1*this->db().time().value()));
#};
}
\endverbatim
See also
Foam::dynamicCode
Foam::functionEntries::codeStream
finiteVolume/fields/fvPatchFields/derived/codedMixed
Constructs on-the-fly a new boundary condition (derived from
mixedFvPatchField) which is then used to evaluate.
Usage
Example:
\verbatim
{
type codedMixed;
refValue uniform (0 0 0);
refGradient uniform (0 0 0);
valueFraction uniform 1;
name rampedMixed; // name of generated BC
code
#{
this->refValue() =
vector(1, 0, 0)
*min(10, 0.1*this->db().time().value());
this->refGrad() = Zero;
this->valueFraction() = 1.0;
#};
//codeInclude
//#{
// #include "fvCFD.H"
//#};
//codeOptions
//#{
// -I$(LIB_SRC)/finiteVolume/lnInclude
//#};
}
\endverbatim
A special form is if the 'code' section is not supplied. In this case
the code gets read from a (runTimeModifiable!) dictionary system/codeDict
which would have a corresponding entry
\verbatim
{
code
#{
this->refValue() = min(10, 0.1*this->db().time().value());
this->refGrad() = Zero;
this->valueFraction() = 1.0;
#};
}
\endverbatim
See also
Foam::dynamicCode
Foam::functionEntries::codeStream
finiteVolume/fields/fvPatchFields/derived/cylindricalInletVelocity
This boundary condition describes an inlet vector boundary condition in
cylindrical co-ordinates given a central axis, central point, rpm, axial
and radial velocity.
Usage
\table
Property | Description | Required | Default value
axis | axis of rotation | yes |
centre | centre of rotation | yes |
axialVelocity | axial velocity profile [m/s] | yes |
radialVelocity | radial velocity profile [m/s] | yes |
rpm | rotational speed (revolutions per minute) | yes|
\endtable
Example of the boundary condition specification:
\verbatim
{
type cylindricalInletVelocity;
axis (0 0 1);
centre (0 0 0);
axialVelocity constant 30;
radialVelocity constant -10;
rpm constant 100;
}
\endverbatim
Note
The \c axialVelocity, \c radialVelocity and \c rpm entries are Function1
types, able to describe time varying functions. The example above gives
the usage for supplying constant values.
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/externalCoupledMixed
This boundary condition provides an interface to an external application.
Values are transferred as plain text files, where OpenFOAM data is written
as:
\verbatim
# Patch:
...
\endverbatim
and received as the constituent pieces of the `mixed' condition, i.e.
\verbatim
# Patch:
...
\endverbatim
Data is sent/received as a single file for all patches from the directory
\verbatim
$FOAM_CASE/
\endverbatim
At start-up, the boundary creates a lock file, i.e..
\verbatim
OpenFOAM.lock
\endverbatim
... to signal the external source to wait. During the boundary condition
update, boundary values are written to file, e.g.
\verbatim
.out
\endverbatim
The lock file is then removed, instructing the external source to take
control of the program execution. When ready, the external program
should create the return values, e.g. to file
\verbatim
.in
\endverbatim
... and then re-instate the lock file. The boundary condition will then
read the return values, and pass program execution back to OpenFOAM.
Usage
\table
Property | Description | Required | Default value
commsDir | communications directory | yes |
fileName | transfer file name | yes |
waitInterval | interval [s] between file checks | no | 1
timeOut | time after which error invoked [s] |no |100*waitInterval
calcFrequency | calculation frequency | no | 1
initByExternal | external app to initialises values | yes |
log | log program control | no | no
\endtable
Example of the boundary condition specification:
\verbatim
{
type externalCoupled;
commsDir "$FOAM_CASE/comms";
fileName data;
calcFrequency 1;
initByExternal yes;
}
\endverbatim
See also
mixedFvPatchField
finiteVolume/fields/fvPatchFields/derived/fan
This boundary condition provides a jump condition, using the \c cyclic
condition as a base.
The jump is specified as a \c Function1 type, to enable the use of, e.g.
contant, polynomial, table values.
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclic| yes |
jumpTable | jump data, e.g. \c csvFile | yes |
phi | flux field name | no | phi
rho | density field name | no | none
\endtable
Example of the boundary condition specification:
\verbatim
{
type fan;
patchType cyclic;
jumpTable csvFile;
csvFileCoeffs
{
hasHeaderLine 1;
refColumn 0;
componentColumns 1(1);
separator ",";
fileName "$FOAM_CASE/constant/pressureVsU";
}
value uniform 0;
}
\endverbatim
The above example shows the use of a comma separated (CSV) file to specify
the jump condition.
Note
The underlying \c patchType should be set to \c cyclic
See also
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/fanPressure
This boundary condition can be applied to assign either a pressure inlet
or outlet total pressure condition for a fan.
Usage
\table
Property | Description | Required | Default value
fileName | fan curve file name | yes |
outOfBounds | out of bounds handling | yes |
direction | direction of flow through fan [in/out] | yes |
p0 | environmental total pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
inlet
{
type fanPressure;
fileName "fanCurve";
outOfBounds clamp;
direction in;
p0 uniform 0;
value uniform 0;
}
outlet
{
type fanPressure;
fileName "fanCurve";
outOfBounds clamp;
direction out;
p0 uniform 0;
value uniform 0;
}
\endverbatim
See also
Foam::fanFvPatchField
Foam::totalPressureFvPatchScalarField
Foam::interpolationTable
finiteVolume/fields/fvPatchFields/derived/fixedFluxExtrapolatedPressure
This boundary condition sets the pressure gradient to the provided value
such that the flux on the boundary is that specified by the velocity
boundary condition.
Example of the boundary condition specification:
\verbatim
{
type fixedFluxExtrapolatedPressure;
}
\endverbatim
See also
Foam::fixedGradientFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedFluxPressure
This boundary condition sets the pressure gradient to the provided value
such that the flux on the boundary is that specified by the velocity
boundary condition.
Example of the boundary condition specification:
\verbatim
{
type fixedFluxPressure;
}
\endverbatim
See also
Foam::fixedGradientFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedInternalValueFvPatchField
This boundary condition provides a mechanism to set boundary (cell) values
directly into a matrix, i.e. to set a constraint condition. Default
behaviour is to act as a zero gradient condition.
Usage
Example of the boundary condition specification:
\verbatim
{
type fixedInternalValue;
value uniform 0; // place holder
}
\endverbatim
Note
This is used as a base for conditions such as the turbulence \c epsilon
wall function, which applies a near-wall constraint for high Reynolds
number flows.
See also
Foam::epsilonWallFunctionFvPatchScalarField
finiteVolume/fields/fvPatchFields/derived/fixedJump
This boundary condition provides a jump condition, using the \c cyclic
condition as a base.
The jump is specified as a fixed value field, applied as an offset to the
'owner' patch.
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclic| yes |
jump | current jump value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedJump;
patchType cyclic;
jump uniform 10;
}
\endverbatim
The above example shows the use of a fixed jump of '10'.
Note
The underlying \c patchType should be set to \c cyclic
See also
Foam::jumpCyclicFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedJumpAMI
This boundary condition provides a jump condition, across non-conformal
cyclic path-pairs, employing an arbitraryMeshInterface (AMI).
The jump is specified as a fixed value field, applied as an offset to the
'owner' patch.
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclic| yes |
jump | current jump value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedJumpAMI;
patchType cyclic;
jump uniform 10;
}
\endverbatim
The above example shows the use of a fixed jump of '10'.
Note
The underlying \c patchType should be set to \c cyclicAMI
See also
Foam::jumpCyclicAMIFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedMean
This boundary condition extrapolates field to the patch using the near-cell
values and adjusts the distribution to match the specified, optionally
time-varying, mean value.
Usage
\table
Property | Description | Required | Default value
meanValue | mean value Function1 | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedMean;
meanValue 1.0;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/fixedNormalInletOutletVelocity
This velocity inlet/outlet boundary condition combines a fixed normal
component obtained from the "normalVelocity" patchField supplied with a
fixed or zero-gradiented tangential component depending on the direction
of the flow and the setting of "fixTangentialInflow":
- Outflow: apply zero-gradient condition to tangential components
- Inflow:
- fixTangentialInflow is true
apply value provided by the normalVelocity patchField to the
tangential components
- fixTangentialInflow is false
apply zero-gradient condition to tangential components.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
fixTangentialInflow | If true fix the tangential component for inflow | yes |
normalVelocity | patchField providing the normal velocity field | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedNormalInletOutletVelocity;
fixTangentialInflow false;
normalVelocity
{
type uniformFixedValue;
uniformValue sine;
uniformValueCoeffs
{
frequency 1;
amplitude table
(
(0 0)
(2 0.088)
(8 0.088)
);
scale (0 1 0);
level (0 0 0);
}
}
value uniform (0 0 0);
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/fixedNormalSlip
This boundary condition sets the patch-normal component to a fixed value.
Usage
\table
Property | Description | Required | Default value
fixedValue | fixed value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedNormalSlip;
fixedValue uniform 0; // example entry for a scalar field
}
\endverbatim
See also
Foam::transformFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedPressureCompressibleDensity
This boundary condition calculates a (liquid) compressible density as a
function of pressure and fluid properties:
\f[
\rho = \rho_{l,sat} + \psi_l*(p - p_{sat})
\f]
where
\vartable
\rho | density [kg/m3]
\rho_{l,sat} | saturation liquid density [kg/m3]
\psi_l | liquid compressibility
p | pressure [Pa]
p_{sat} | saturation pressure [Pa]
\endvartable
The variables \c rholSat, \c pSat and \c psil are retrieved from the
\c thermodynamicProperties dictionary.
Usage
\table
Property | Description | Required | Default value
p | pressure field name | no | p
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedPressureCompressibleDensity;
p p;
value uniform 1;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/fixedProfile
This boundary condition provides a fixed value profile condition.
Usage
\table
Property | Description | Required | Default value
profile | Profile Function1 | yes |
direction | Profile direction | yes |
origin | Profile origin | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedProfile;
profile csvFile;
profileCoeffs
{
nHeaderLine 0; // Number of header lines
refColumn 0; // Reference column index
componentColumns (1 2 3); // Component column indices
separator ","; // Optional (defaults to ",")
mergeSeparators no; // Merge multiple separators
fileName "Uprofile.csv"; // name of csv data file
outOfBounds clamp; // Optional out-of-bounds handling
interpolationScheme linear; // Optional interpolation scheme
}
direction (0 1 0);
origin 0;
}
\endverbatim
Example setting a parabolic inlet profile for the PitzDaily case:
\verbatim
inlet
{
type fixedProfile;
profile polynomial
(
((1 0 0) (0 0 0))
((-6200 0 0) (2 0 0))
);
direction (0 1 0);
origin 0.0127;
}
\endverbatim
Note
The profile entry is a Function1 type. The example above gives the
usage for supplying csv file.
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
Foam::timeVaryingMappedFixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/flowRateInletVelocity
This boundary condition provides a velocity boundary condition, derived
from the flux (volumetric or mass-based), whose direction is assumed
to be normal to the patch.
For a mass-based flux:
- the flow rate should be provided in kg/s
- if \c rho is "none" the flow rate is in m3/s
- otherwise \c rho should correspond to the name of the density field
- if the density field cannot be found in the database, the user must
specify the inlet density using the \c rhoInlet entry
For a volumetric-based flux:
- the flow rate is in m3/s
Usage
\table
Property | Description | Required | Default value
massFlowRate | mass flow rate [kg/s] | no |
volumetricFlowRate | volumetric flow rate [m3/s]| no |
rhoInlet | inlet density | no |
extrapolateProfile | Extrapolate velocity profile | no | false
\endtable
Example of the boundary condition specification for a volumetric flow rate:
\verbatim
{
type flowRateInletVelocity;
volumetricFlowRate 0.2;
extrapolateProfile yes;
value uniform (0 0 0);
}
\endverbatim
Example of the boundary condition specification for a mass flow rate:
\verbatim
{
type flowRateInletVelocity;
massFlowRate 0.2;
extrapolateProfile yes;
rho rho;
rhoInlet 1.0;
value uniform (0 0 0);
}
\endverbatim
The \c flowRate entry is a \c Function1 of time, see Foam::Function1Types.
Note
- \c rhoInlet is required for the case of a mass flow rate, where the
density field is not available at start-up
- The value is positive into the domain (as an inlet)
- May not work correctly for transonic inlets
- Strange behaviour with potentialFoam since the U equation is not solved
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/fluxCorrectedVelocity
This boundary condition provides a velocity outlet boundary condition for
patches where the pressure is specified. The outflow velocity is obtained
by "zeroGradient" and then corrected from the flux:
\f[
U_p = U_c - n (n \cdot U_c) + \frac{n \phi_p}{|S_f|}
\f]
where
\vartable
U_p | velocity at the patch [m/s]
U_c | velocity in cells adjacent to the patch [m/s]
n | patch normal vectors
\phi_p | flux at the patch [m3/s or kg/s]
S_f | patch face area vectors [m2]
\endvartable
where
\table
Property | Description | Required | Default value
phi | name of flux field | no | phi
rho | name of density field | no | rho
\endtable
Example of the boundary condition specification:
\verbatim
{
type fluxCorrectedVelocity;
phi phi;
rho rho;
}
\endverbatim
Note
If reverse flow is possible or expected use the
pressureInletOutletVelocity condition instead.
See also
Foam::zeroGradientFvPatchField
Foam::pressureInletOutletVelocityFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/freestream
This boundary condition provides a free-stream condition. It is a 'mixed'
condition derived from the \c inletOutlet condition, whereby the mode of
operation switches between fixed (free stream) value and zero gradient
based on the sign of the flux.
Usage
\table
Property | Description | Required | Default value
freestreamValue | freestream velocity | yes |
phi | flux field name | no | phi
\endtable
Example of the boundary condition specification:
\verbatim
{
type freestream;
phi phi;
}
\endverbatim
See also
Foam::mixedFvPatchField
Foam::inletOutletFvPatchField
finiteVolume/fields/fvPatchFields/derived/freestreamPressure
This boundary condition provides a free-stream condition for pressure.
It is a zero-gradient condition that constrains the flux across the patch
based on the free-stream velocity.
Usage
\table
Property | Description | Required | Default value
U | velocity field name | no | U
phi | flux field name | no | phi
rho | density field name | no | none
\endtable
Example of the boundary condition specification:
\verbatim
{
type freestreamPressure;
}
\endverbatim
Note
This condition is designed to operate with a freestream velocity condition
See also
Foam::zeroGradientFvPatchField
Foam::freestreamFvPatchField
finiteVolume/fields/fvPatchFields/derived/inletOutlet
This boundary condition provides a generic outflow condition, with
specified inflow for the case of return flow.
Usage
\table
Property | Description | Required | Default value
phi | Flux field name | no | phi
inletValue | Inlet value for reverse flow | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type inletOutlet;
phi phi;
inletValue uniform 0;
value uniform 0;
}
\endverbatim
The mode of operation is determined by the sign of the flux across the
patch faces.
Note
Sign conventions:
- Positive flux (out of domain): apply zero-gradient condition
- Negative flux (into of domain): apply the "inletValue" fixed-value
See also
Foam::mixedFvPatchField
Foam::zeroGradientFvPatchField
Foam::outletInletFvPatchField
finiteVolume/fields/fvPatchFields/derived/inletOutletTotalTemperature
This boundary condition provides an outflow condition for total
temperature for use with supersonic cases, where a user-specified
value is applied in the case of reverse flow.
Usage
\table
Property | Description | Required | Default value
U | velocity field name | no | U
phi | flux field name | no | phi
psi | compressibility field name | no | psi
gamma | heat capacity ration (Cp/Cv) | yes |
inletValue | reverse flow (inlet) value | yes |
T0 | static temperature [K] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type inletOutletTotalTemperature;
U U;
phi phi;
psi psi;
gamma gamma;
inletValue uniform 0;
T0 uniform 0;
value uniform 0;
}
\endverbatim
See also
Foam::inletOutletFvPatchField
finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity
Inlet velocity in which the actual interstitial velocity is calculated
by dividing the specified inletVelocity field with the local phase-fraction.
Example of the boundary condition specification:
\verbatim
inlet
{
type interstitialInletVelocity;
inletVelocity uniform (0 0.2 0);// Non-interstitial inlet velocity
alpha alpha.particles; // Name of the phase-fraction field
value uniform (0 0 0);
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/mappedField
This boundary condition provides a self-contained version of the \c mapped
condition. It does not use information on the patch; instead it holds
thr data locally.
Usage
\table
Property | Description | Required | Default value
fieldName | name of field to be mapped | no | this field name
setAverage | flag to activate setting of average value | yes |
average | average value to apply if \c setAverage = yes | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type mappedField;
fieldName T; // optional field name
setAverage no; // apply an average value
average 0; // average to apply if setAverage
value uniform 0; // place holder
}
\endverbatim
Note
Since this condition can be applied on a per-field and per-patch basis,
it is possible to duplicate the mapping information. If possible, employ
the \c mapped condition in preference to avoid this situation, and only
employ this condition if it is not possible to change the underlying
geometric (poly) patch type to \c mapped.
See also
Foam::mappedPatchBase
Foam::mappedPolyPatch
Foam::mappedFvPatch
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/mappedFixedInternalValue
This boundary condition maps the boundary and internal values of a
neighbour patch field to the boundary and internal values of *this.
Usage
\table
Property | Description | Required | Default value
fieldName | name of field to be mapped | no | this field name
setAverage | flag to activate setting of average value | yes |
average | average value to apply if \c setAverage = yes | yes |
\endtable
\verbatim
{
type mappedFixedInternalValue;
fieldName T;
setAverage no;
average 0;
value uniform 0;
}
\endverbatim
Note
This boundary condition can only be applied to patches that are of
the \c mappedPolyPatch type.
See also
Foam::mappedPatchBase
Foam::mappedPolyPatch
Foam::mappedFvPatch
Foam::mappedFixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/mappedFixedPushedInternalValue
This boundary condition maps the boundary values of a neighbour patch
field to the boundary and internal cell values of *this.
Usage
\table
Property | Description | Required | Default value
fieldName | name of field to be mapped | no | this field name
setAverage | flag to activate setting of average value | yes |
average | average value to apply if \c setAverage = yes | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type mappedFixedPushedInternalValue;
fieldName T;
setAverage no;
average 0;
value uniform 0;
}
\endverbatim
Note
This boundary condition can only be applied to patches that are of
the \c mappedPolyPatch type.
See also
Foam::mappedPatchBase
Foam::mappedPolyPatch
Foam::mappedFvPatch
Foam::mappedFixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/mappedFixedValue
This boundary condition maps the value at a set of cells or patch faces
back to *this.
The sample mode is set by the underlying mapping engine, provided by the
mappedPatchBase class.
Usage
\table
Property | Description | Required | Default value
fieldName | name of field to be mapped | no | this field name
setAverage | flag to activate setting of average value | yes |
average | average value to apply if \c setAverage = yes | yes |
interpolationScheme | type of interpolation scheme | no |
\endtable
Example of the boundary condition specification:
\verbatim
{
type mapped;
fieldName T;
setAverage no;
average 0;
interpolationScheme cell;
value uniform 0;
}
\endverbatim
When employing the \c nearestCell sample mode, the user must also specify
the interpolation scheme using the \c interpolationScheme entry.
In case of interpolation (where scheme != cell) the limitation is that
there is only one value per cell. For example, if you have a cell with two
boundary faces and both faces sample into the cell, both faces will get the
same value.
Note
It is not possible to sample internal faces since volume fields are not
defined on faces.
See also
Foam::mappedPatchBase
Foam::interpolation
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/mappedFlowRate
Describes a volumetric/mass flow normal vector boundary condition by its
magnitude as an integral over its area.
The inlet mass flux is taken from the neighbour region.
The basis of the patch (volumetric or mass) is determined by the
dimensions of the flux, phi. The current density is used to correct the
velocity when applying the mass basis.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
neigPhi | name of flux field on neighbour mesh | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type mappedFlowRate;
phi phi;
rho rho;
neigPhi phi;
value uniform (0 0 0); // placeholder
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/mappedVelocityFluxFixedValue
This boundary condition maps the velocity and flux from a neighbour patch
to this patch
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
\endtable
Example of the boundary condition specification:
\verbatim
{
type mappedVelocityFlux;
phi phi;
value uniform 0; // place holder
}
\endverbatim
The underlying sample mode should be set to \c nearestPatchFace or
\c nearestFace
Note
This boundary condition can only be applied to patches that are of
the \c mappedPolyPatch type.
See also
Foam::mappedPatchBase
Foam::mappedPolyPatch
Foam::mappedFvPatch
Foam::fixedValueFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/movingWallVelocity
This boundary condition provides a velocity condition for cases with
moving walls.
Usage
Example of the boundary condition specification:
\verbatim
{
type movingWallVelocity;
value uniform (0 0 0); // Initial value
}
\endverbatim
See also
Foam::fixedValueFvPatchVectorField
Foam::MRFZone
finiteVolume/fields/fvPatchFields/derived/noSlip
This boundary condition fixes the velocity to zero at walls.
Usage
Example of the boundary condition specification:
\verbatim
{
type noSlip;
}
\endverbatim
See also
Foam::fixedValueFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/outletInlet
This boundary condition provides a generic inflow condition, with
specified outflow for the case of reverse flow.
Usage
\table
Property | Description | Required | Default value
phi | Flux field name | no | phi
outletValue | Outlet value for reverse flow | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type outletInlet;
phi phi;
outletValue uniform 0;
value uniform 0;
}
\endverbatim
The mode of operation is determined by the sign of the flux across the
patch faces.
Note
Sign conventions:
- Positive flux (out of domain): apply the "outletValue" fixed-value
- Negative flux (into of domain): apply zero-gradient condition
See also
Foam::mixedFvPatchField
Foam::zeroGradientFvPatchField
Foam::inletOutletFvPatchField
finiteVolume/fields/fvPatchFields/derived/outletMappedUniformInlet
This boundary conditon averages the field over the "outlet" patch specified
by name "outletPatchName" and applies this as the uniform value of the
field over this patch.
Usage
\table
Property | Description | Required | Default value
outletPatchName | name of outlet patch | yes |
phi | flux field name | no | phi
\endtable
Example of the boundary condition specification:
\verbatim
{
type outletMappedUniformInlet;
outletPatchName aPatch;
phi phi;
value uniform 0;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/outletPhaseMeanVelocity
This boundary condition adjusts the velocity for the given phase to achieve
the specified mean thus causing the phase-fraction to adjust according to
the mass flow rate.
Typical usage is as the outlet condition for a towing-tank ship simulation
to maintain the outlet water level at the level as the inlet.
Usage
\table
Property | Description | Required | Default value
Umean | mean velocity normal to the boundary [m/s] | yes |
alpha | phase-fraction field | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type outletPhaseMeanVelocity;
Umean 1.2;
alpha alpha.water;
value uniform (1.2 0 0);
}
\endverbatim
See also
Foam::mixedFvPatchField
Foam::variableHeightFlowRateInletVelocityFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/partialSlip
This boundary condition provides a partial slip condition. The amount of
slip is controlled by a user-supplied field.
Usage
\table
Property | Description | Required | Default value
valueFraction | fraction od value used for boundary [0-1] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type partialSlip;
valueFraction uniform 0.1;
value uniform 0;
}
\endverbatim
See also
Foam::transformFvPatchField
finiteVolume/fields/fvPatchFields/derived/phaseHydrostaticPressure
This boundary condition provides a phase-based hydrostatic pressure
condition, calculated as:
\f[
p_{hyd} = p_{ref} + \rho g (x - x_{ref})
\f]
where
\vartable
p_{hyd} | hyrostatic pressure [Pa]
p_{ref} | reference pressure [Pa]
x_{ref} | reference point in Cartesian co-ordinates
\rho | density (assumed uniform)
g | acceleration due to gravity [m/s2]
\endtable
The values are assigned according to the phase-fraction field:
- 1: apply \$fp_{hyd}\$f
- 0: apply a zero-gradient condition
Usage
\table
Property | Description | Required | Default value
phaseFraction | phase-fraction field name | no | alpha
rho | density field name | no | rho
pRefValue | reference pressure [Pa] | yes |
pRefPoint | reference pressure location | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type phaseHydrostaticPressure;
phaseFraction alpha1;
rho rho;
pRefValue 1e5;
pRefPoint (0 0 0);
value uniform 0; // optional initial value
}
\endverbatim
See also
Foam::mixedFvPatchScalarField
finiteVolume/fields/fvPatchFields/derived/plenumPressure
This boundary condition provides a plenum pressure inlet condition. This
condition creates a zero-dimensional model of an enclosed volume of gas
upstream of the inlet. The pressure that the boundary condition exerts on
the inlet boundary is dependent on the thermodynamic state of the upstream
volume. The upstream plenum density and temperature are time-stepped along
with the rest of the simulation, and momentum is neglected. The plenum is
supplied with a user specified mass flow and temperature.
The result is a boundary condition which blends between a pressure inlet
condition condition and a fixed mass flow. The smaller the plenum
volume, the quicker the pressure responds to a deviation from the supply
mass flow, and the closer the model approximates a fixed mass flow. As
the plenum size increases, the model becomes more similar to a specified
pressure.
The expansion from the plenum to the inlet boundary is controlled by an
area ratio and a discharge coefficient. The area ratio can be used to
represent further acceleration between a sub-grid blockage such as fins.
The discharge coefficient represents a fractional deviation from an
ideal expansion process.
This condition is useful for simulating unsteady internal flow problems
for which both a mass flow boundary is unrealistic, and a pressure
boundary is susceptible to flow reversal. It was developed for use in
simulating confined combustion.
Reference:
\verbatim
Bainbridge, W. (2013).
The Numerical Simulation of Oscillations in Gas Turbine Combustion
Chambers,
PhD Thesis,
Chapter 4, Section 4.3.1.2, 77-80.
\endverbatim
Usage
\table
Property | Description | Required | Default value
gamma | ratio of specific heats | yes | none
R | specific gas constant | yes | none
supplyMassFlowRate | flow rate into the plenum | yes | none
supplyTotalTemperature | temperature into the plenum | yes | none
plenumVolume | plenum volume | yes | none
plenumDensity | plenum density | yes | none
plenumTemperature | plenum temperature | yes | none
U | velocity field name | no | U
phi | flux field name | no | phi
rho | inlet density | no | none
inletAreaRatio | inlet open fraction | yes | none
inletDischargeCoefficient | inlet loss coefficient | yes | none
timeScale | relaxation time scale | yes | none
\endtable
Example of the boundary condition specification:
\verbatim
{
type plenumPressure;
gamma 1.4;
R 287.04;
supplyMassFlowRate 0.0001;
supplyTotalTemperature 300;
plenumVolume 0.000125;
plenumDensity 1.1613;
plenumTemperature 300;
inletAreaRatio 1.0;
inletDischargeCoefficient 0.8;
timeScale 1e-4;
value uniform 1e5;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/pressureDirectedInletOutletVelocity
This velocity inlet/outlet boundary condition is applied to pressure
boundaries where the pressure is specified. A zero-gradient condtion is
applied for outflow (as defined by the flux); for inflow, the velocity
is obtained from the flux with the specified inlet direction.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
inletDirection | inlet direction per patch face | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type pressureDirectedInletOutletVelocity;
phi phi;
rho rho;
inletDirection uniform (1 0 0);
value uniform 0;
}
\endverbatim
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux with specified
direction
See also
Foam::mixedFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/pressureDirectedInletVelocity
This velocity inlet boundary condition is applied to patches where the
pressure is specified. The inflow velocity is obtained from the flux with
the specified inlet direction" direction.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
inletDirection | inlet direction per patch face | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type pressureDirectedInletVelocity;
phi phi;
rho rho;
inletDirection uniform (1 0 0);
value uniform 0;
}
\endverbatim
Note
If reverse flow is possible or expected use the
pressureDirectedInletOutletVelocityFvPatchVectorField condition instead.
See also
Foam::fixedValueFvPatchField
Foam::pressureDirectedInletOutletVelocityFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/pressureInletOutletParSlipVelocity
This velocity inlet/outlet boundary condition for pressure boundary where
the pressure is specified. A zero-gradient is applied for outflow (as
defined by the flux); for inflow, the velocity is obtained from the flux
with the specified inlet direction.
A slip condition is applied tangential to the patch.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
\endtable
Example of the boundary condition specification:
\verbatim
{
type pressureInletOutletParSlipVelocity;
value uniform 0;
}
\endverbatim
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux with specified
direction
See also
Foam::mixedFvPatchVectorField
Foam::pressureDirectedInletOutletVelocityFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/pressureInletOutletVelocity
This velocity inlet/outlet boundary condition is applied to pressure
boundaries where the pressure is specified. A zero-gradient condition is
applied for outflow (as defined by the flux); for inflow, the velocity is
obtained from the patch-face normal component of the internal-cell value.
The tangential patch velocity can be optionally specified.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
tangentialVelocity | tangential velocity field | no |
\endtable
Example of the boundary condition specification:
\verbatim
{
type pressureInletOutletVelocity;
phi phi;
tangentialVelocity uniform (0 0 0);
value uniform 0;
}
\endverbatim
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux in the patch-normal
direction
finiteVolume/fields/fvPatchFields/derived/pressureInletUniformVelocity
This velocity inlet boundary condition is applied to patches where the
pressure is specified. The uniform inflow velocity is obtained by
averaging the flux over the patch, and then applying it in the direction
normal to the patch faces.
Usage
Example of the boundary condition specification:
\verbatim
{
type pressureInletUniformVelocity;
value uniform 0;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/pressureInletVelocity
This velocity inlet boundary condition is applied to patches where the
pressure is specified. The inflow velocity is obtained from the flux with
a direction normal to the patch faces.
Usage
Example of the boundary condition specification:
\verbatim
{
type pressureInletVelocity;
phi phi;
rho rho;
value uniform 0;
}
\endverbatim
Note
If reverse flow is possible or expected use
the pressureInletOutletVelocityFvPatchVectorField condition instead.
See also
Foam::fixedValueFvPatchField
Foam::pressureInletOutletVelocityFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/pressureNormalInletOutletVelocity
This velocity inlet/outlet boundary condition is applied to patches where
the pressure is specified. A zero-gradient condition is applied for
outflow (as defined by the flux); for inflow, the velocity is obtained from
the flux with a direction normal to the patch faces.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
\endtable
Example of the boundary condition specification:
\verbatim
{
type pressureNormalInletOutletVelocity;
phi phi;
rho rho;
value uniform 0;
}
\endverbatim
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux and patch-normal
direction
See also
Foam::mixedFvPatchVectorField
finiteVolume/fields/fvPatchFields/derived/prghPressure
This boundary condition provides static pressure condition for p_rgh,
calculated as:
\f[
p_rgh = p - \rho g (h - hRef)
\f]
where
\vartable
p_rgh | Pseudo hydrostatic pressure [Pa]
p | Static pressure [Pa]
h | Height in the opposite direction to gravity
hRef | Reference height in the opposite direction to gravity
\rho | density
g | acceleration due to gravity [m/s^2]
\endtable
Usage
\table
Property | Description | Required | Default value
rho | rho field name | no | rho
p | static pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type prghPressure;
rho rho;
p uniform 0;
value uniform 0; // optional initial value
}
\endverbatim
See also
Foam::fixedValueFvPatchScalarField
finiteVolume/fields/fvPatchFields/derived/prghTotalHydrostaticPressure
This boundary condition provides static pressure condition for p_rgh,
calculated as:
\f[
p_rgh = ph_rgh - 0.5 \rho |U|^2
\f]
where
\vartable
p_rgh | Pressure - \rho g.(h - hRef) [Pa]
ph_rgh | Hydrostatic pressure - \rho g.(h - hRef) [Pa]
h | Height in the opposite direction to gravity
hRef | Reference height in the opposite direction to gravity
\rho | Density
g | Acceleration due to gravity [m/s^2]
\endtable
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
ph_rgh | ph_rgh field name | no | ph_rgh
value | Patch face values | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type prghTotalHydrostaticPressure;
value uniform 0;
}
\endverbatim
See also
Foam::fixedValueFvPatchScalarField
Foam::prghTotalPressureFvPatchScalarField
finiteVolume/fields/fvPatchFields/derived/prghTotalPressure
This boundary condition provides static pressure condition for p_rgh,
calculated as:
\f[
p_rgh = p - \rho g.(h - hRef)
p = p0 - 0.5 \rho |U|^2
\f]
where
\vartable
p_rgh | Pseudo hydrostatic pressure [Pa]
p | Static pressure [Pa]
p0 | Total pressure [Pa]
h | Height in the opposite direction to gravity
hRef | Reference height in the opposite direction to gravity
\rho | Density
g | Acceleration due to gravity [m/s^2]
\endtable
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
p0 | Total pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type prghTotalPressure;
p0 uniform 0;
}
\endverbatim
See also
Foam::fixedValueFvPatchScalarField
finiteVolume/fields/fvPatchFields/derived/rotatingPressureInletOutletVelocity
This velocity inlet/outlet boundary condition is applied to patches in a
rotating frame where the pressure is specified. A zero-gradient is applied
for outflow (as defined by the flux); for inflow, the velocity is obtained
from the flux with a direction normal to the patch faces.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
tangentialVelocity | tangential velocity field | no |
omega | angular velocty of the frame [rad/s] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type rotatingPressureInletOutletVelocity;
phi phi;
tangentialVelocity uniform (0 0 0);
omega 100;
}
\endverbatim
The \c omega entry is a Function1 type, able to describe time varying
functions.
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): derive from the flux in the patch-normal
direction
See also
Foam::pressureInletOutletVelocityFvPatchVectorField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/rotatingTotalPressure
This boundary condition provides a total pressure condition for patches
in a rotating frame.
Usage
\table
Property | Description | Required | Default value
U | velocity field name | no | U
phi | flux field name | no | phi
rho | density field name | no | none
psi | compressibility field name | no | none
gamma | ratio of specific heats (Cp/Cv) | yes |
p0 | static pressure reference | yes |
omega | angular velocty of the frame [rad/s] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type rotatingTotalPressure;
U U;
phi phi;
rho rho;
psi psi;
gamma 1.4;
p0 uniform 1e5;
omega 100;
}
\endverbatim
The \c omega entry is a Function1 type, able to describe time varying
functions.
See also
Foam::totalPressureFvPatchScalarField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/rotatingWallVelocity
This boundary condition provides a rotational velocity condition.
Usage
\table
Property | Description | Required | Default value
origin | origin of rotation in Cartesian co-ordinates | yes|
axis | axis of rotation | yes |
omega | angular velocty of the frame [rad/s] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type rotatingWallVelocity;
origin (0 0 0);
axis (0 0 1);
omega 100;
}
\endverbatim
The \c omega entry is a Function1 of time, see Foam::Function1Types.
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/slip
This boundary condition provides a slip constraint.
Usage
Example of the boundary condition specification:
\verbatim
{
type slip;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/supersonicFreestream
This boundary condition provides a supersonic free-stream condition.
- supersonic outflow is vented according to ???
- supersonic inflow is assumed to occur according to the Prandtl-Meyer
expansion process.
- subsonic outflow is applied via a zero-gradient condition from inside
the domain.
Usage
\table
Property | Description | Required | Default value
T | Temperature field name | no | T
p | Pressure field name | no | p
psi | Compressibility field name | no | thermo:psi
UInf | free-stream velocity | yes |
pInf | free-stream pressure | yes |
TInf | free-stream temperature | yes |
gamma | heat capacity ratio (cp/Cv) | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type supersonicFreestream;
UInf 500;
pInf 1e4;
TInf 265;
gamma 1.4;
}
\endverbatim
Note
This boundary condition is ill-posed if the free-stream flow is normal
to the boundary.
finiteVolume/fields/fvPatchFields/derived/surfaceNormalFixedValue
This boundary condition provides a surface-normal vector boundary condition
by its magnitude.
Usage
\table
Property | Description | Required | Default value
refValue | reference value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type surfaceNormalFixedValue;
refValue uniform -10; // 10 INTO the domain
}
\endverbatim
Note
Sign conventions:
- the value is positive for outward-pointing vectors
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/swirlFlowRateInletVelocity
This boundary condition provides a volumetric- OR mass-flow normal vector
boundary condition by its magnitude as an integral over its area with a
swirl component determined by the angular speed, given in revolutions per
minute (RPM)
The basis of the patch (volumetric or mass) is determined by the
dimensions of the flux, phi. The current density is used to correct the
velocity when applying the mass basis.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
flowRate | flow rate profile | yes |
rpm | rotational speed profile | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type swirlFlowRateInletVelocity;
flowRate constant 0.2;
rpm constant 100;
}
\endverbatim
Note
- the \c flowRate and \c rpm entries are Function1 types, able to describe
time varying functions. The example above gives the usage for supplying
constant values.
- the value is positive into the domain
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/syringePressure
This boundary condition provides a pressure condition, obtained from a
zero-D model of the cylinder of a syringe.
The syringe cylinder is defined by its initial volume, piston area and
velocity profile specified by regions of constant acceleration, speed
and deceleration. The gas in the cylinder is described by its initial
pressure and compressibility which is assumed constant, i.e. isothermal
expansion/compression.
Usage
\table
Property | Description | Required | Default value
Ap | syringe piston area [m2] | yes |
Sp | syringe piston speed [m/s] | yes |
VsI | initial syringe volume [m3] | yes |
tas | start of piston acceleration [s] | yes |
tae | end of piston acceleration [s] | yes |
tds | start of piston deceleration [s] | yes |
tde | end of piston deceleration [s] | yes |
psI | initial syringe pressure [Pa] | yes |
psi | gas compressibility [m2/s2] | yes |
ams | added (or removed) gas mass [kg] | yes |
\endtable
Example of the BC specification:
\verbatim
{
type syringePressure;
Ap 1.388e-6;
Sp 0.01;
VsI 1.388e-8;
tas 0.001;
tae 0.002;
tds 0.005;
tde 0.006;
psI 1e5;
psi 1e-5;
ams 0;
value uniform 0;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/timeVaryingMappedFixedValue
This boundary conditions interpolates the values from a set of supplied
points in space and time. Supplied data should be specified in
constant/boundaryData/\ where:
- points : pointField with locations
- ddd : supplied values at time ddd
The default mode of operation (mapMethod planarInterpolation) is
to project the points onto a plane (constructed from the first threee
points) and construct a 2D triangulation and finds for the face centres
the triangle it is in and the weights to the 3 vertices.
The optional mapMethod nearest will avoid all projection and
triangulation and just use the value at the nearest vertex.
Values are interpolated linearly between times.
Usage
\table
Property | Description | Required | Default value
setAverage | flag to activate setting of average value | yes |
perturb | perturb points for regular geometries | no | 1e-5
fieldTableName | alternative field name to sample | no| this field name
mapMethod | type of mapping | no | planarInterpolation
offset | for applying offset to mapped values | no | constant 0.0
\endtable
\verbatim
{
type timeVaryingMappedFixedValue;
setAverage false;
//perturb 0.0;
//fieldTableName samples;
//offset constant 0.2;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/totalPressure
This boundary condition provides a total pressure condition. Four
variants are possible:
1. incompressible subsonic:
\f[
p_p = p_0 - 0.5 |U|^2
\f]
where
\vartable
p_p | incompressible pressure at patch [m2/s2]
p_0 | incompressible total pressure [m2/s2]
U | velocity
\endvartable
2. compressible subsonic:
\f[
p_p = p_0 - 0.5 \rho |U|^2
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | total pressure [Pa]
\rho | density [kg/m3]
U | velocity
\endvartable
3. compressible transonic (\f$\gamma = 1\f$):
\f[
p_p = \frac{p_0}{1 + 0.5 \psi |U|^2}
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | total pressure [Pa]
G | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
\endvartable
4. compressible supersonic (\f$\gamma > 1\f$):
\f[
p_p = \frac{p_0}{(1 + 0.5 \psi G |U|^2)^{\frac{1}{G}}}
\f]
where
\vartable
p_p | pressure at patch [Pa]
p_0 | total pressure [Pa]
\gamma | ratio of specific heats (Cp/Cv)
\psi | compressibility [m2/s2]
G | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
\endvartable
The modes of operation are set by the dimensions of the pressure field
to which this boundary condition is applied, the \c psi entry and the value
of \c gamma:
\table
Mode | dimensions | psi | gamma
incompressible subsonic | p/rho | |
compressible subsonic | p | none |
compressible transonic | p | psi | 1
compressible supersonic | p | psi | > 1
\endtable
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
psi | Compressibility field name | no | none
gamma | (Cp/Cv) | no | 1
p0 | Total pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type totalPressure;
p0 uniform 1e5;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/totalTemperature
This boundary condition provides a total temperature condition.
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
psi | Compressibility field name | no | thermo:psi
gamma | ratio of specific heats (Cp/Cv) | yes |
T0 | reference temperature | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type totalTemperature;
T0 uniform 300;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/translatingWallVelocity
This boundary condition provides a velocity condition for translational
motion on walls.
Usage
\table
Property | Description | Required | Default value
U | translational velocity | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type translatingWallVelocity;
U (100 0 0);
}
\endverbatim
The \c U entry is a Function1 of time, see Foam::Function1Types.
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/turbulentInlet
This boundary condition generates a fluctuating inlet condition by adding
a random component to a reference (mean) field.
\f[
x_p = (1 - \alpha) x_p^{n-1} + \alpha (x_{ref} + s C_{RMS} x_{ref})
\f]
where
\vartable
x_p | patch values
x_{ref} | reference patch values
n | time level
\alpha | fraction of new random component added to previous time value
C_{RMS} | RMS coefficient
s | fluctuation scale
\endvartable
Usage
\table
Property | Description | Required | Default value
fluctuationScale | RMS fluctuation scale (fraction of mean) | yes |
referenceField | reference (mean) field | yes |
alpha | fraction of new random component added to previous| no| 0.1
\endtable
Example of the boundary condition specification:
\verbatim
{
type turbulentInlet;
fluctuationScale 0.1;
referenceField uniform 10;
alpha 0.1;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/turbulentIntensityKineticEnergyInlet
This boundary condition provides a turbulent kinetic energy condition,
based on user-supplied turbulence intensity, defined as a fraction of the
mean velocity:
\f[
k_p = 1.5 (I |U|)^2
\f]
where
\vartable
k_p | kinetic energy at the patch
I | turbulence intensity
U | velocity field
\endvartable
In the event of reverse flow, a zero-gradient condition is applied.
Usage
\table
Property | Description | Required | Default value
intensity | fraction of mean field [0-1] | yes |
U | velocity field name | no | U
phi | flux field name | no | phi
\endtable
Example of the boundary condition specification:
\verbatim
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05; // 5% turbulence
value uniform 1; // placeholder
}
\endverbatim
See also
Foam::inletOutletFvPatchField
finiteVolume/fields/fvPatchFields/derived/uniformDensityHydrostaticPressure
This boundary condition provides a hydrostatic pressure condition,
calculated as:
\f[
p_{hyd} = p_{ref} + \rho g (x - x_{ref})
\f]
where
\vartable
p_{hyd} | hyrostatic pressure [Pa]
p_{ref} | reference pressure [Pa]
x_{ref} | reference point in Cartesian co-ordinates
\rho | density (assumed uniform)
g | acceleration due to gravity [m/s2]
\endtable
Usage
\table
Property | Description | Required | Default value
rho | uniform density [kg/m3] | yes |
pRefValue | reference pressure [Pa] | yes |
pRefPoint | reference pressure location | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformDensityHydrostaticPressure;
rho rho;
pRefValue 1e5;
pRefPoint (0 0 0);
value uniform 0; // optional initial value
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/uniformFixedGradient
This boundary condition provides a uniform fixed gradient condition.
Usage
\table
Property | Description | Required | Default value
uniformGradient | uniform gradient | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformFixedGradient;
uniformGradient constant 0.2;
}
\endverbatim
Note
The uniformGradient entry is a Function1 type, able to describe time
varying functions. The example above gives the usage for supplying a
constant value.
See also
Foam::Function1Types
Foam::fixedGradientFvPatchField
finiteVolume/fields/fvPatchFields/derived/uniformFixedValue
This boundary condition provides a uniform fixed value condition.
Usage
\table
Property | Description | Required | Default value
uniformValue | uniform value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformFixedValue;
uniformValue constant 0.2;
}
\endverbatim
Note
The uniformValue entry is a Function1 type, able to describe time
varying functions. The example above gives the usage for supplying a
constant value.
See also
Foam::Function1Types
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/uniformInletOutlet
Variant of inletOutlet boundary condition with uniform inletValue.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
uniformInletValue | inlet value for reverse flow | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformInletOutlet;
phi phi;
uniformInletValue 0;
value uniform 0;
}
\endverbatim
The mode of operation is determined by the sign of the flux across the
patch faces.
Note
Sign conventions:
- positive flux (out of domain): apply zero-gradient condition
- negative flux (into of domain): apply the user-specified fixed value
See also
Foam::inletOutletFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/uniformJump
This boundary condition provides a jump condition, using the \c cyclic
condition as a base. The jump is specified as a time-varying uniform
value across the patch.
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclic| yes |
jumpTable | jump value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformJump;
patchType cyclic;
jumpTable constant 10;
}
\endverbatim
The above example shows the use of a fixed jump of '10'.
Note
The uniformValue entry is a Function1 type, able to describe time
varying functions. The example above gives the usage for supplying a
constant value.
The underlying \c patchType should be set to \c cyclic
See also
Foam::fixedJumpFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/uniformJumpAMI
This boundary condition provides a jump condition, using the \c cyclicAMI
condition as a base. The jump is specified as a time-varying uniform
value across the patch.
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclicAMI| yes |
jumpTable | jump value | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformJumpAMI;
patchType cyclicAMI;
jumpTable constant 10;
}
\endverbatim
The above example shows the use of a fixed jump of '10'.
Note
The uniformValue entry is a Function1 type, able to describe time
varying functions. The example above gives the usage for supplying a
constant value.
The underlying \c patchType should be set to \c cyclic
See also
Foam::jumpCyclicAMIFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/uniformTotalPressure
This boundary condition provides a time-varying form of the uniform total
pressure boundary condition Foam::totalPressureFvPatchField.
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
psi | Compressibility field name | no | none
gamma | (Cp/Cv) | no | 1
p0 | Total pressure as a function of time | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type uniformTotalPressure;
p0 uniform 1e5;
}
\endverbatim
The \c p0 entry is specified as a Function1 type, able to describe
time varying functions.
See also
Foam::Function1Types
Foam::uniformFixedValueFvPatchField
Foam::totalPressureFvPatchField
finiteVolume/fields/fvPatchFields/derived/variableHeightFlowRate
This boundary condition provides a phase fraction condition based on the
local flow conditions, whereby the values are constrained to lay between
user-specified upper and lower bounds. The behaviour is described by:
if alpha > upperBound:
- apply a fixed value condition, with a uniform level of the upper bound
if lower bound <= alpha <= upper bound:
- apply a zero-gradient condition
if alpha < lowerBound:
- apply a fixed value condition, with a uniform level of the lower bound
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
lowerBound | lower bound for clipping | yes |
upperBound | upper bound for clipping | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type variableHeightFlowRate;
lowerBound 0.0;
upperBound 0.9;
value uniform 0;
}
\endverbatim
finiteVolume/fields/fvPatchFields/derived/variableHeightFlowRateInletVelocity
This boundary condition provides a velocity boundary condition for
multphase flow based on a user-specified volumetric flow rate.
The flow rate is made proportional to the phase fraction alpha at each
face of the patch and alpha is ensured to be bound between 0 and 1.
Usage
\table
Property | Description | Required | Default value
flowRate | volumetric flow rate [m3/s] | yes |
alpha | phase-fraction field | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type variableHeightFlowRateInletVelocity;
flowRate 0.2;
alpha alpha.water;
value uniform (0 0 0); // placeholder
}
\endverbatim
The \c flowRate entry is a \c Function1 of time, see Foam::Function1Types.
Note
- the value is positive into the domain
- may not work correctly for transonic inlets
- strange behaviour with potentialFoam since the momentum equation is
not solved
See also
Foam::fixedValueFvPatchField
Foam::Function1Types
finiteVolume/fields/fvPatchFields/derived/waveSurfacePressure
This is a pressure boundary condition, whose value is calculated as
the hydrostatic pressure based on a given displacement:
\f[
p = -\rho*g*\zeta
\f]
\vartable
\rho | density [kg/m3]
g | acceleration due to gravity [m/s2]
\zeta | wave amplitude [m]
\endvartable
The wave amplitude is updated as part of the calculation, derived from the
local volumetric flux.
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
zeta | wave amplitude field name | no | zeta
\endtable
Example of the boundary condition specification:
\verbatim
{
type waveSurfacePressure;
phi phi;
rho rho;
zeta zeta;
value uniform 0; // place holder
}
\endverbatim
The density field is only required if the flux is mass-based as opposed to
volumetric-based.
See also
Foam::fixedValueFvPatchField
finiteVolume/fields/fvPatchFields/derived/waveTransmissive
This boundary condition provides a wave transmissive outflow condition,
based onsolving DDt(psi, U) = 0 at the boundary.
The wave speed is calculated using:
\f[
x_p = \frac{\phi_p}{|Sf|} + \sqrt{\frac{\gamma}{\psi_p}}
\f]
where
\vartable
x_p | patch values
\phi_p | patch face flux
\psi_p | patch compressibility
Sf | patch face area vector
\gamma | ratio of specific heats
\endvartable
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
psi | compressibility field name | no | psi
gamma | ratio of specific heats (Cp/Cv) | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type waveTransmissive;
phi phi;
psi psi;
gamma 1.4;
}
\endverbatim
See also
Foam::advectiveFvPatchField
fvMotionSolver/fvPatchFields/derived/cellMotion
Foam::cellMotionFvPatchField
fvMotionSolver/fvPatchFields/derived/surfaceSlipDisplacement
fvPatchField corresponding to surfaceSlipDisplacementPointPatchField.
Is just a slip type since all hard work (projection) is done in the
pointPatch field.
genericPatchFields/genericFvPatchField
This boundary condition provides a generic version of the \c calculated
condition, useful as a fallback for handling unknown patch types. Not
generally applicable as a user-specified condition.
See also
Foam::calculatedFvPatchField
regionCoupled/derivedFvPatchFields/energyRegionCoupled
Energy region coupled implicit boundary condition.
The fvPatch is treated as uncoupled from the delta point of view.
In the mesh the fvPatch is an interface and is incorporated
into the matrix implicitly.
regionModels/regionCoupling/derivedFvPatchFields/filmPyrolysisRadiativeCoupledMixed
Mixed boundary condition for temperature, to be used in the flow and
pyrolysis regions when a film region model is used.
Example usage:
\verbatim
myInterfacePatchName
{
type filmPyrolysisRadiativeCoupledMixed;
Tnbr T;
kappa fluidThermo;
Qr Qr;
kappaName none;
filmDeltaDry 0.0;
filmDeltaWet 3e-4;
value $internalField;
}
\endverbatim
Needs to be on underlying mapped(Wall)FvPatch.
It calculates local field as:
\verbatim
ratio = (filmDelta - filmDeltaDry)/(filmDeltaWet - filmDeltaDry)
\endverbatim
when ratio = 1 is considered wet and the film temperature is fixed at
the wall. If ratio = 0 (dry) it emulates the normal radiative solid BC.
In between ratio 0 and 1 the gradient and value contributions are
weighted using the ratio field in the following way:
\verbatim
qConv = ratio*htcwfilm*(Tfilm - *this);
qRad = (1.0 - ratio)*Qr;
\endverbatim
Then the solid can gain or loose energy through radiation or conduction
towards the film.
Notes:
- kappa and \c kappaName are inherited from temperatureCoupledBase.
- Qr is the radiative flux defined in the radiation model.
See also
Foam::temperatureCoupledBase
regionModels/regionCoupling/derivedFvPatchFields/filmPyrolysisTemperatureCoupled
This boundary condition is designed to be used in conjunction with surface
film and pyrolysis modelling. It provides a temperature boundary condition
for patches on the primary region based on whether the patch is seen to
be 'wet', retrieved from the film alpha field.
- if the patch is wet, the temperature is set using the film temperature
- otherwise, it is set using pyrolysis temperature
Example of the boundary condition specification:
\verbatim
{
type filmPyrolysisTemperatureCoupled;
phi phi; // name of flux field (default = phi)
rho rho; // name of density field (default = rho)
deltaWet 1e-4; // threshold height for 'wet' film
value uniform 300; // initial temperature / [K]
}
\endverbatim
regionModels/regionCoupling/derivedFvPatchFields/filmPyrolysisVelocityCoupled
This boundary condition is designed to be used in conjunction with surface
film and pyrolysis modelling.
It provides a velocity boundary condition for patches on the primary region
based on whether the patch is seen to be 'wet', retrieved from the film
alpha field.
- if the patch is wet, the velocity is set using the film velocity
- otherwise, it is set using pyrolysis out-gassing velocity
Example of the boundary condition specification:
\verbatim
{
type filmPyrolysisVelocityCoupled;
phi phi; // name of flux field (default = phi)
rho rho; // name of density field (default = rho)
deltaWet 1e-4; // threshold height for 'wet' film
value uniform (0 0 0); // initial velocity / [m/s]
}
\endverbatim
regionModels/surfaceFilmModels/derivedFvPatchFields/filmHeightInletVelocity
This boundary condition is designed to be used in conjunction with
surface film modelling. It provides a velocity inlet boundary condition
for patches where the film height is specified. The inflow velocity is
obtained from the flux with a direction normal to the patch faces using:
\f[
U_p = \frac{n \phi}{\rho |Sf| \delta}
\f]
where
\vartable
U_p | patch velocity [m/s]
n | patch normal vector
\phi | mass flux [kg/s]
\rho | density [kg/m3]
Sf | patch face area vectors [m2]
\delta | film height [m]
\endvartable
Usage
\table
Property | Description | Required | Default value
phi | Flux field name | no | phi
rho | density field name | no | rho
deltaf | height field name | no | deltaf
\endtable
Example of the boundary condition specification:
\verbatim
{
type filmHeightInletVelocity;
phi phi;
rho rho;
deltaf deltaf;
value uniform (0 0 0); // initial velocity / [m/s]
}
\endverbatim
See also
Foam::fixedValueFvPatchField
regionModels/surfaceFilmModels/derivedFvPatchFields/inclinedFilmNusseltHeight
Film height boundary condition for inclined films that imposes a
sinusoidal perturbation on top of a mean flow rate, where the height is
calculated using the Nusselt solution.
regionModels/surfaceFilmModels/derivedFvPatchFields/inclinedFilmNusseltInletVelocity
Film velocity boundary condition for inclined films that imposes a
sinusoidal perturbation on top of a mean flow rate, where the velocity is
calculated using the Nusselt solution.
regionModels/surfaceFilmModels/derivedFvPatchFields/wallFunctions/alphatFilmWallFunction
This boundary condition provides a turbulent thermal diffusivity condition
when using wall functions, for use with surface film models. This
condition varies from the standard wall function by taking into account any
mass released from the film model.
Usage
\table
Property | Description | Required | Default value
B | model coefficient | no | 5.5
yPlusCrit | critical y+ for transition to turbulent flow | no|11.05
Cmu | model coefficient | no | 0.09
kappa | Von-Karman constant | no | 0.41
Prt | turbulent Prandtl number | no | 0.85
\endtable
Example of the boundary condition specification:
\verbatim
{
type alphatFilmWallFunction;
B 5.5;
yPlusCrit 11.05;
Cmu 0.09;
kappa 0.41;
Prt 0.85;
value uniform 0;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
regionModels/surfaceFilmModels/derivedFvPatchFields/wallFunctions/nutkFilmWallFunction
This boundary condition provides a turbulent viscosity condition when
using wall functions, based on turbulence kinetic energy, for use with
surface film models.
Usage
Example of the boundary condition specification:
\verbatim
{
type nutkFilmWallFunction;
value uniform 0;
}
\endverbatim
See also
Foam::nutkWallFunctionFvPatchScalarField
regionModels/thermalBaffleModels/derivedFvPatchFields/thermalBaffle
This boundary condition provides a coupled temperature condition between
multiple mesh regions.
The regions are generally referred to as the:
- primary region,
- and baffle region.
The primary region creates the baffle region and evolves its energy
equation either:
- 1-D, normal to each patch face
- 2-D, normal and tangential components
The thermodynamic properties of the baffle material are specified via
dictionary entries on the master patch.
Usage
Example of the boundary condition specification:
\verbatim
{
type compressible::thermalBaffle;
// Underlaying coupled boundary condition
Tnbr T;
kappa fluidThermo; // or solidThermo
KappaName none;
QrNbr Qr;//or none.Name of Qr field on neighbourregion
Qr none;// or none.Name of Qr field on localregion
value uniform 300;
// Baffle region name
regionName baffleRegion;
active yes;
// Solid thermo in solid region
thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}
mixture
{
specie
{
nMoles 1;
molWeight 20;
}
transport
{
kappa 0.01;
}
thermodynamics
{
Hf 0;
Cp 15;
}
density
{
rho 80;
}
}
radiation
{
radiationModel opaqueSolid;
absorptionEmissionModel none;
scatterModel none;
}
// Extrude model for new region
extrudeModel linearNormal;
nLayers 50;
expansionRatio 1;
columnCells false; //3D or 1D
linearNormalCoeffs
{
thickness 0.02;
}
}
\endverbatim
Slave patch on primary region:
\verbatim
{
type compressible::thermalBaffle;
kappa fluidThermo;
kappaName none;
value uniform 300;
\endverbatim
Patches on baffle region:
\verbatim
bottom
{
type compressible::thermalBaffle;
kappa solidThermo;
kappaName none;
value uniform 300;
}
top
{
type compressible::thermalBaffle;
kappa solidThermo;
kappaName none;
value uniform 300;
}
\endverbatim
See also
Foam::compressible::turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
Foam::regionModels::thermalBaffleModels::thermalBaffleModel
thermophysicalModels/basic/derivedFvPatchFields/energyJump/energyJump
This boundary condition provides an energy jump condition across a pair
of coupled patches. It is not applied directly, but is employed on-the-fly
when converting temperature boundary conditions into energy.
See also
Foam::fixedJumpFvPatchField
thermophysicalModels/basic/derivedFvPatchFields/energyJump/energyJumpAMI
This boundary condition provides an energy jump condition across a pair
of coupled patches with an arbitrary mesh interface (AMI). It is not
applied directly, but is employed on-the-fly when converting temperature
boundary conditions into energy.
See also
Foam::fixedJumpAMIFvPatchField
thermophysicalModels/basic/derivedFvPatchFields/fixedEnergy
This boundary condition provides a fixed condition for internal energy
Usage
Example of the boundary condition specification:
\verbatim
{
type fixedEnergy;
value uniform 100;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
thermophysicalModels/basic/derivedFvPatchFields/gradientEnergy
This boundary condition provides a gradient condition for internal energy,
where the gradient is calculated using:
\f[
\nabla(e_p) = \nabla_\perp C_p(p, T) + \frac{e_p - e_c}{\Delta}
\f]
where
\vartable
e_p | energy at patch faces [J]
e_c | energy at patch internal cells [J]
p | pressure [bar]
T | temperature [K]
C_p | specific heat [J/kg/K]
\Delta | distance between patch face and internal cell centres [m]
\endvartable
Usage
Example of the boundary condition specification:
\verbatim
{
type gradientEnergy;
gradient uniform 10;
}
\endverbatim
See also
Foam::fixedGradientFvPatchField
thermophysicalModels/basic/derivedFvPatchFields/mixedEnergy
This boundary condition provides a mixed condition for internal energy
See also
Foam::mixedFvPatchField
thermophysicalModels/radiation/derivedFvPatchFields/greyDiffusiveRadiation
This boundary condition provides a grey-diffuse condition for radiation
intensity, \c I, for use with the finite-volume discrete-ordinates model
(fvDOM), in which the radiation temperature is retrieved from the
temperature field boundary condition.
Usage
\table
Property | Description | Required | Default value
T | temperature field name | no | T
emissivityMode | emissivity mode: solidRadiation or lookup | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type greyDiffusiveRadiation;
T T;
emissivityMode solidRadiation;
value uniform 0;
}
\endverbatim
See also
Foam::radiationCoupledBase
Foam::radiation::radiationModel
Foam::radiation::fvDOM
Foam::mixedFvPatchField
thermophysicalModels/radiation/derivedFvPatchFields/greyDiffusiveViewFactor
This boundary condition provides a grey-diffuse condition for radiative
heat flux, \c Qr, for use with the view factor model
Usage
\table
Property | Description | Required | Default value
Qro | external radiative heat flux | yes |
emissivityMode | emissivity mode: solidRadiation or lookup | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type greyDiffusiveRadiationViewFactor;
Qro uniform 0;
emissivityMode solidRadiation;
value uniform 0;
}
\endverbatim
See also
Foam::radiationCoupledBase
Foam::radiation::radiationModel
Foam::radiation::viewFactor
Foam::fixedValueFvPatchField
thermophysicalModels/radiation/derivedFvPatchFields/MarshakRadiation
A 'mixed' boundary condition that implements a Marshak condition for the
incident radiation field (usually written as G)
The radiation temperature is retrieved from the mesh database, using a
user specified temperature field name.
Usage
\table
Property | Description | Required | Default value
T | temperature field name | no | T
\endtable
Example of the boundary condition specification:
\verbatim
{
type MarshakRadiation;
T T;
value uniform 0;
}
\endverbatim
See also
Foam::radiationCoupledBase
Foam::mixedFvPatchField
thermophysicalModels/radiation/derivedFvPatchFields/MarshakRadiationFixedTemperature
A 'mixed' boundary condition that implements a Marshak condition for the
incident radiation field (usually written as G)
The radiation temperature field across the patch is supplied by the user
using the \c Trad entry.
Usage
\table
Property | Description | Required | Default value
T | temperature field name | no | T
\endtable
Example of the boundary condition specification:
\verbatim
{
type MarshakRadiationFixedTemperature;
Trad uniform 1000; // radiation temperature field
value uniform 0; // place holder
}
\endverbatim
See also
Foam::radiationCoupledBase
Foam::mixedFvPatchField
thermophysicalModels/radiation/derivedFvPatchFields/wideBandDiffusiveRadiation
This boundary condition provides a wide-band, diffusive radiation
condition, where the patch temperature is specified.
Usage
\table
Property | Description | Required | Default value
T | temperature field name | no | T
\endtable
Example of the boundary condition specification:
\verbatim
{
type wideBandDiffusiveRadiation;
value uniform 0;
}
\endverbatim
See also
Foam::mixedFvPatchScalarField
Foam::radiationCoupledBase
thermophysicalModels/reactionThermo/derivedFvPatchFields/fixedUnburntEnthalpy
Fixed boundary condition for unburnt
thermophysicalModels/reactionThermo/derivedFvPatchFields/gradientUnburntEnthalpy
gradient boundary condition for unburnt
thermophysicalModels/reactionThermo/derivedFvPatchFields/mixedUnburntEnthalpy
Mixed boundary condition for unburnt
transportModels/twoPhaseProperties/alphaContactAngle/alphaContactAngle
Abstract base class for alphaContactAngle boundary conditions.
Derived classes must implement the theta() fuction which returns the
wall contact angle field.
The essential entry "limit" controls the gradient of alpha1 on the wall:
- none - Calculate the gradient from the contact-angle without limiter
- gradient - Limit the wall-gradient such that alpha1 remains bounded
on the wall
- alpha - Bound the calculated alpha1 on the wall
- zeroGradient - Set the gradient of alpha1 to 0 on the wall, i.e.
reproduce previous behaviour, the pressure BCs can be left as before.
Note that if any of the first three options are used the boundary condition
on \c p_rgh must set to guarantee that the flux is corrected to be zero at
the wall e.g.:
\verbatim
{
type alphaContactAngle;
limit none;
}
\endverbatim
transportModels/twoPhaseProperties/alphaContactAngle/constantAlphaContactAngle
A constant alphaContactAngle scalar boundary condition.
See also
Foam::alphaContactAngleFvPatchScalarField
Foam::temperatureDependentAlphaContactAngleFvPatchScalarField
transportModels/twoPhaseProperties/alphaContactAngle/dynamicAlphaContactAngle
A dynamic alphaContactAngle scalar boundary condition
(alphaContactAngleFvPatchScalarField)
transportModels/twoPhaseProperties/alphaContactAngle/temperatureDependentAlphaContactAngle
Temperature-dependent constant alphaContactAngle scalar boundary condition.
Usage
\table
Property | Description | Required | Default value
T | Temperature field name | no | T
theta0 | Contact angle data | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type temperatureDependentAlphaContactAngle;
theta0 constant 60;
}
\endverbatim
See also
Foam::alphaContactAngleFvPatchScalarField
Foam::constantAlphaContactAngleFvPatchScalarField
transportModels/twoPhaseProperties/alphaContactAngle/timeVaryingAlphaContactAngle
A time-varying alphaContactAngle scalar boundary condition
(alphaContactAngleFvPatchScalarField)
transportModels/twoPhaseProperties/alphaFixedPressure
A fixed-pressure alphaContactAngle boundary
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/convectiveHeatTransfer
This boundary condition provides a convective heat transfer coefficient
condition
if Re > 500000
\f[
htc_p = \frac{0.664 Re^{0.5} Pr^{0.333} \kappa_p}{L}
\f]
else
\f[
htc_p = \frac{0.037 Re^{0.8} Pr^{0.333} \kappa_p}{L}
\f]
where
\vartable
htc_p | patch convective heat transfer coefficient
Re | Reynolds number
Pr | Prandtl number
\kappa_p | thermal conductivity
L | length scale
\endvartable
Usage
\table
Property | Description | Required | Default value
L | Length scale [m] | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type convectiveHeatTransfer;
L 0.1;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/externalCoupledTemperatureMixed
This boundary condition provides a temperature interface to an external
application. Values are transferred as plain text files, where OpenFOAM
data is written as:
\verbatim
# Patch:
...
\endverbatim
and received as the constituent pieces of the `mixed' condition, i.e.
\verbatim
# Patch:
...
\endverbatim
Data is sent/received as a single file for all patches from the directory
\verbatim
$FOAM_CASE/
\endverbatim
At start-up, the boundary creates a lock file, i.e..
\verbatim
OpenFOAM.lock
\endverbatim
... to signal the external source to wait. During the boundary condition
update, boundary values are written to file, e.g.
\verbatim
.out
\endverbatim
The lock file is then removed, instructing the external source to take
control of the program execution. When ready, the external program
should create the return values, e.g. to file
\verbatim
.in
\endverbatim
... and then re-instate the lock file. The boundary condition will then
read the return values, and pass program execution back to OpenFOAM.
Usage
\table
Property | Description | Required | Default value
commsDir | communications directory | yes |
fileName | transfer file name | yes |
waitInterval | interval [s] between file checks | no | 1
timeOut | time after which error invoked [s] |no |100*waitInterval
calcFrequency | calculation frequency | no | 1
log | log program control | no | no
\endtable
Example of the boundary condition specification:
\verbatim
{
type externalCoupledTemperature;
commsDir "$FOAM_CASE/comms";
fileName data;
calcFrequency 1;
}
\endverbatim
See also
mixedFvPatchField
externalCoupledMixedFvPatchField
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/externalWallHeatFluxTemperature
This boundary condition supplies a heat flux condition for temperature
on an external wall. Optional thin thermal layer resistances can be
specified through thicknessLayers and kappaLayers entries for the
fixed heat transfer coefficient mode.
The condition can operate in two modes:
- fixed heat transfer coefficient: supply h and Ta
- fixed heat flux: supply q
where:
\vartable
h | heat transfer coefficient [W/m^2/K]
Ta | ambient temperature [K]
q | heat flux [W/m^2]
\endvartable
The thermal conductivity \c kappa can either be retrieved from various
possible sources, as detailed in the class temperatureCoupledBase.
Usage
\table
Property | Description | Required | Default value
q | heat flux [W/m^2] | yes* |
Ta | ambient temperature [K] | yes* |
h | heat transfer coefficient [W/m^2/K] | yes*|
thicknessLayers | list of thicknesses per layer [m] | yes |
kappaLayers | list of thermal conductivities per layer [W/m/K] | yes |
Qr | name of the radiative field | no | no
relaxation | relaxation factor for radiative field | no | 1
kappaMethod | inherited from temperatureCoupledBase | inherited |
kappa | inherited from temperatureCoupledBase | inherited |
\endtable
Example of the boundary condition specification:
\verbatim
{
type externalWallHeatFluxTemperature;
q uniform 1000;
Ta uniform 300.0;
h uniform 10.0;
thicknessLayers (0.1 0.2 0.3 0.4);
kappaLayers (1 2 3 4);
value uniform 300.0;
Qr none;
relaxation 1;
kappaMethod fluidThermo;
kappa none;
}
\endverbatim
Note:
- Only supply \c h and \c Ta, or \c q in the dictionary (see above)
See also
Foam::temperatureCoupledBase
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/thermalBaffle1D
This BC solves a steady 1D thermal baffle.
The solid properties are specify as dictionary. Optionaly radiative heat
flux (Qr) can be incorporated into the balance. Some under-relaxation might
be needed on Qr. Baffle and solid properties need to be specified on the
master side of the baffle.
Usage
Example of the boundary condition specification using constant
solid thermo :
\verbatim
{
type compressible::thermalBaffle1D;
samplePatch ;
thickness uniform 0.005; // thickness [m]
Qs uniform 100; // heat flux [W/m2]
Qr none;
relaxation 1;
// Solid thermo
specie
{
nMoles 1;
molWeight 20;
}
transport
{
kappa 1;
}
thermodynamics
{
Hf 0;
Cp 10;
}
equationOfState
{
rho 10;
}
value uniform 300;
}
{
type compressible::thermalBaffle1D;
samplePatch ;
Qr none;
relaxation 1;
}
\endverbatim
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/totalFlowRateAdvectiveDiffusive
This BC is used for species inlets. The diffusion and advection fluxes are
considered to calculate the inlet value for the species
The massFluxFraction sets the fraction of the flux of each particular
species.
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/turbulentHeatFluxTemperature
Fixed heat boundary condition to specify temperature gradient. Input
heat source either specified in terms of an absolute power [W], or as a
flux [W/m^2].
The thermal conductivity \c kappa can either be retrieved from various
possible sources, as detailed in the class temperatureCoupledBase.
Usage
\table
Property | Description | Required | Default value
heatSource | 'power' [W] or 'flux' [W/m^2] | yes |
q | heat power or flux field | yes |
Qr | name of the radiative flux field | yes |
value | initial temperature value | no | calculated
gradient | initial gradient value | no | 0.0
kappaMethod | inherited from temperatureCoupledBase | inherited |
kappa | inherited from temperatureCoupledBase | inherited |
\endtable
Note: If needed, both 'value' and 'gradient' must be defined to be used.
Example usage:
\verbatim
hotWall
{
type compressible::turbulentHeatFluxTemperature;
heatSource flux;
q uniform 10;
kappaMethod fluidThermo;
kappa none;
Qr none;
}
\endverbatim
See also
Foam::temperatureCoupledBase
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/turbulentTemperatureCoupledBaffleMixed
Mixed boundary condition for temperature, to be used for heat-transfer
on back-to-back baffles. Optional thin thermal layer resistances can be
specified through thicknessLayers and kappaLayers entries.
Specifies gradient and temperature such that the equations are the same
on both sides:
- refGradient = zero gradient
- refValue = neighbour value
- mixFraction = nbrKDelta / (nbrKDelta + myKDelta())
where KDelta is heat-transfer coefficient K * deltaCoeffs
The thermal conductivity \c kappa can either be retrieved from various
possible sources, as detailed in the class temperatureCoupledBase.
Usage
\table
Property | Description | Required | Default value
Tnbr | name of the field | no | T
thicknessLayers | list of thicknesses per layer [m] | no |
kappaLayers | list of thermal conductivities per layer [W/m/K] | no |
kappaMethod | inherited from temperatureCoupledBase | inherited |
kappa | inherited from temperatureCoupledBase | inherited |
\endtable
Example of the boundary condition specification:
\verbatim
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
Tnbr T;
thicknessLayers (0.1 0.2 0.3 0.4);
kappaLayers (1 2 3 4);
kappaMethod lookup;
kappa kappa;
value uniform 300;
}
\endverbatim
Needs to be on underlying mapped(Wall)FvPatch.
See also
Foam::temperatureCoupledBase
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/turbulentTemperatureRadCoupledMixed
Mixed boundary condition for temperature and radiation heat transfer
to be used for in multiregion cases. Optional thin thermal layer
resistances can be specified through thicknessLayers and kappaLayers
entries.
The thermal conductivity \c kappa can either be retrieved from various
possible sources, as detailed in the class temperatureCoupledBase.
Usage
\table
Property | Description | Required | Default value
Tnbr | name of the field | no | T
QrNbr | name of the radiative flux in the nbr region | no | none
Qr | name of the radiative flux in this region | no | none
thicknessLayers | list of thicknesses per layer [m] | no |
kappaLayers | list of thermal conductivites per layer [W/m/K] | no |
kappaMethod | inherited from temperatureCoupledBase | inherited |
kappa | inherited from temperatureCoupledBase | inherited |
\endtable
Example of the boundary condition specification:
\verbatim
{
type compressible::turbulentTemperatureRadCoupledMixed;
Tnbr T;
QrNbr Qr; // or none. Name of Qr field on neighbour region
Qr Qr; // or none. Name of Qr field on local region
thicknessLayers (0.1 0.2 0.3 0.4);
kappaLayers (1 2 3 4);
kappaMethod lookup;
kappa kappa;
value uniform 300;
}
\endverbatim
Needs to be on underlying mapped(Wall)FvPatch.
See also
Foam::temperatureCoupledBase
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatJayatillekeWallFunction
This boundary condition provides a thermal wall function for turbulent
thermal diffusivity (usually\c alphat) based on the Jayatilleke model.
Usage
\table
Property | Description | Required | Default value
Prt | turbulent Prandtl number | no | 0.85
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type alphatJayatillekeWallFunction;
Prt 0.85;
kappa 0.41;
E 9.8;
value uniform 0; // optional value entry
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatPhaseChangeWallFunction
Abstract base-class for all alphatWallFunctions supporting phase-change.
See also
Foam::fixedValueFvPatchScalarField
Foam::alphatWallFunctionFvPatchScalarField
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatWallFunction
This boundary condition provides a turbulent thermal diffusivity conditon
when using wall functions
- replicates OpenFOAM v1.5 (and earlier) behaviour
The turbulent thermal diffusivity calculated using:
\f[
\alpha_t = \frac{\mu_t}{Pr_t}
\f]
where
\vartable
\alpha_t| turblence thermal diffusivity
\mu_t | turblence viscosity
Pr_t | turblent Prandtl number
\endvartable
Usage
\table
Property | Description | Required | Default value
nut | turbulence viscosity field name | no | nut
Prt | turbulent Prandtl number | no | 0.85
\endtable
Example of the boundary condition specification:
\verbatim
{
type alphatWallFunction;
nut nut;
Prt 0.85;
value uniform 0; // optional value entry
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/wallHeatTransfer
This boundary condition provides an enthalpy condition for wall heat
transfer
Usage
\table
Property | Description | Required | Default value
Tinf | wall temperature | yes |
alphaWall | thermal diffusivity | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type wallHeatTransfer;
Tinf uniform 500;
alphaWall uniform 1;
}
\endverbatim
TurbulenceModels/incompressible/turbulentTransportModels/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatJayatillekeWallFunction
This boundary condition provides a kinematic turbulent thermal conductivity
for using wall functions, using the Jayatilleke 'P' function.
Usage
\table
Property | Description | Required | Default value
Prt | turbulent Prandtl number | no | 0.85
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type alphatJayatillekeWallFunction;
}
\endverbatim
Note
The units of kinematic turbulent thermal conductivity are [m2/s]
See also
Foam::fixedValueFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/fixedShearStress
Set a constant shear stress as tau0 = -nuEff dU/dn.
TurbulenceModels/turbulenceModels/derivedFvPatchFields/porousBafflePressure
This boundary condition provides a jump condition, using the \c cyclic
condition as a base.
The porous baffle introduces a pressure jump defined by:
\f[
\Delta p = -(D \mu U + 0.5 I \rho |U|^2 )L
\f]
where
\vartable
p | pressure [Pa]
\rho | density [kg/m3]
\mu | laminar viscosity [Pa s]
D | Darcy coefficient
I | inertial coefficient
L | porous media length in the flow direction
\endvartable
Usage
\table
Property | Description | Required | Default value
patchType | underlying patch type should be \c cyclic| yes |
phi | flux field name | no | phi
rho | density field name | no | rho
D | Darcy coefficient | yes |
I | inertial coefficient | yes |
length | porous media length in the flow direction | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type porousBafflePressure;
patchType cyclic;
jump uniform 0;
D 0.001;
I 1000000;
length 0.1;
value uniform 0;
}
\endverbatim
Note
The underlying \c patchType should be set to \c cyclic
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/epsilonWallFunctions/epsilonLowReWallFunction
This boundary condition provides a turbulence dissipation wall function
condition for low- and high-Reynolds number turbulent flow cases.
The condition can be applied to wall boundaries, whereby it inserts near
wall epsilon values directly into the epsilon equation to act as a
constraint.
The model operates in two modes, based on the computed laminar-to-turbulent
switch-over y+ value derived from kappa and E.
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type epsilonLowReWallFunction;
}
\endverbatim
See also
Foam::epsilonWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/epsilonWallFunctions/epsilonWallFunction
This boundary condition provides a turbulence dissipation wall function
condition for high Reynolds number, turbulent flow cases.
The condition can be applied to wall boundaries, whereby it
- calculates \c epsilon and \c G
- inserts near wall epsilon values directly into the epsilon equation
to act as a constraint
where
\vartable
epsilon | turblence dissipation field
G | turblence generation field
\endvartable
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type epsilonWallFunction;
}
\endverbatim
See also
Foam::fixedInternalValueFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/fWallFunctions/fWallFunction
This boundary condition provides a turbulence damping function, f, wall
function condition for low- and high Reynolds number, turbulent flow cases
The model operates in two modes, based on the computed laminar-to-turbulent
switch-over y+ value derived from kappa and E.
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type fWallFunction;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/kqRWallFunctions/kLowReWallFunction
This boundary condition provides a turbulence kinetic energy wall function
condition for low- and high-Reynolds number turbulent flow cases.
The model operates in two modes, based on the computed laminar-to-turbulent
switch-over y+ value derived from kappa and E.
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
Ceps2 | model coefficient | no | 1.9
\endtable
Example of the boundary condition specification:
\verbatim
{
type kLowReWallFunction;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/kqRWallFunctions/kqRWallFunction
This boundary condition provides a suitable condition for turbulence
\c k, \c q, and \c R fields for the case of high Reynolds number flow using
wall functions.
It is a simple wrapper around the zero-gradient condition.
Usage
Example of the boundary condition specification:
\verbatim
{
type kqRWallFunction;
}
\endverbatim
See also
Foam::zeroGradientFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutkAtmRoughWallFunction
This boundary condition provides a turbulent kinematic viscosity for
atmospheric velocity profiles. It is desinged to be used in conjunction
with the atmBoundaryLayerInletVelocity boundary condition. The values
are calculated using:
\f[
U = frac{U_f}{K} ln(\frac{z + z_0}{z_0})
\f]
where
\vartable
U_f | frictional velocity
K | Von Karman's constant
z_0 | surface roughness length
z | vertical co-ordinate
\endvartable
Usage
\table
Property | Description | Required | Default value
z0 | surface roughness length| yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type nutkAtmRoughWallFunction;
z0 uniform 0;
}
\endverbatim
See also
Foam::nutkWallFunctionFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutkRoughWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions for rough walls, based on turbulence kinetic
energy. The condition manipulates the E parameter to account for roughness
effects.
Parameter ranges
- roughness height = sand-grain roughness (0 for smooth walls)
- roughness constant = 0.5-1.0
Usage
\table
Property | Description | Required | Default value
Ks | sand-grain roughness height | yes |
Cs | roughness constant | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type nutkRoughWallFunction;
Ks uniform 0;
Cs uniform 0.5;
}
\endverbatim
See also
Foam::nutkRoughWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutkWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions, based on turbulence kinetic energy.
- replicates OpenFOAM v1.5 (and earlier) behaviour
Usage
Example of the boundary condition specification:
\verbatim
{
type nutkWallFunction;
}
\endverbatim
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutLowReWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
for use with low Reynolds number models. It sets \c nut to zero, and
provides an access function to calculate y+.
Usage
Example of the boundary condition specification:
\verbatim
{
type nutLowReWallFunction;
}
\endverbatim
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutURoughWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions for rough walls, based on velocity.
Usage
\table
Property | Description | Required | Default value
roughnessHeight | roughness height | yes |
roughnessConstant | roughness constanr | yes |
roughnessFactor | scaling factor | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type nutURoughWallFunction;
roughnessHeight 1e-5;
roughnessConstant 0.5;
roughnessFactor 1;
}
\endverbatim
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUSpaldingWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions for rough walls, based on velocity, using
Spalding's law to give a continuous nut profile to the wall (y+ = 0)
\f[
y^+ = u^+ + \frac{1}{E} \left[exp(\kappa u^+) - 1 - \kappa u^+\,
- 0.5 (\kappa u^+)^2 - \frac{1}{6} (\kappa u^+)^3\right]
\f]
where
\vartable
y^+ | non-dimensional position
u^+ | non-dimensional velocity
\kappa | Von Karman constant
\endvartable
Usage
Example of the boundary condition specification:
\verbatim
{
type nutUSpaldingWallFunction;
}
\endverbatim
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUTabulatedWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions. As input, the user specifies a look-up table
of U+ as a function of near-wall Reynolds number. The table should be
located in the $FOAM_CASE/constant directory.
Usage
\table
Property | Description | Required | Default value
uPlusTable | U+ as a function of Re table name | yes |
\endtable
Example of the boundary condition specification:
\verbatim
{
type nutTabulatedWallFunction;
uPlusTable myUPlusTable;
}
\endverbatim
Note
The tables are not registered since the same table object may be used for
more than one patch.
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions, based on velocity.
Usage
Example of the boundary condition specification:
\verbatim
{
type nutUWallFunction;
}
\endverbatim
See also
Foam::nutWallFunctionFvPatchScalarField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutWallFunction
This boundary condition provides a turbulent kinematic viscosity condition
when using wall functions, based on turbulence kinetic energy.
- replicates OpenFOAM v1.5 (and earlier) behaviour
Usage
\table
Property | Description | Required | Default value
Cmu | Cmu coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | E coefficient | no | 9.8
\endtable
Examples of the boundary condition specification:
\verbatim
{
type nutWallFunction;
value uniform 0.0;
}
\endverbatim
Reference for the default model coefficients:
\verbatim
H. Versteeg, W. Malalasekera
An Introduction to Computational Fluid Dynamics: The Finite Volume
Method, subsection "3.5.2 k-epsilon model"
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/omegaWallFunctions/omegaWallFunction
This boundary condition provides a wall function constraint on turbulnce
specific dissipation, omega. The values are computed using:
\f[
\omega = sqrt(\omega_{vis}^2 + \omega_{log}^2)
\f]
where
\vartable
\omega_{vis} | omega in viscous region
\omega_{log} | omega in logarithmic region
\endvartable
Model described by Eq.(15) of:
\verbatim
Menter, F., Esch, T.
"Elements of Industrial Heat Transfer Prediction"
16th Brazilian Congress of Mechanical Engineering (COBEM),
Nov. 2001
\endverbatim
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
beta1 | model coefficient | no | 0.075
\endtable
Example of the boundary condition specification:
\verbatim
{
type omegaWallFunction;
}
\endverbatim
TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/v2WallFunctions/v2WallFunction
This boundary condition provides a turbulence stress normal to streamlines
wall function condition for low- and high-Reynolds number, turbulent flow
cases.
The model operates in two modes, based on the computed laminar-to-turbulent
switch-over y+ value derived from kappa and E.
Usage
\table
Property | Description | Required | Default value
Cmu | model coefficient | no | 0.09
kappa | Von Karman constant | no | 0.41
E | model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type v2WallFunction;
}
\endverbatim
See also
Foam::fixedValueFvPatchField
TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/atmBoundaryLayerInletEpsilon
This boundary condition specifies an inlet value for the turbulence
dissipation, \f$\epsilon\f$, appropriate for atmospheric boundary layers.
See Foam::atmBoundaryLayer for details.
Example of the boundary condition specification:
\verbatim
ground
{
type atmBoundaryLayerInletEpsilon;
z (0 0 1);
Uref 10.0;
Zref 20.0;
z0 uniform 0.1;
zGround uniform 0.0;
}
\endverbatim
See also
Foam::atmBoundaryLayer,
Foam::atmBoundaryLayerInletVelocityFvPatchVectorField,
Foam::atmBoundaryLayerInletKFvPatchScalarField
TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/atmBoundaryLayerInletK
This boundary condition specifies an inlet value for the turbulence
kinetic energy, \f$k\f$, appropriate for atmospheric boundary layers.
See Foam::atmBoundaryLayer for details.
Example of the boundary condition specification:
\verbatim
ground
{
type atmBoundaryLayerInletK;
z (0 0 1);
Uref 10.0;
Zref 20.0;
z0 uniform 0.1;
zGround uniform 0.0;
}
\endverbatim
See also
Foam::atmBoundaryLayer,
Foam::atmBoundaryLayerInletVelocityFvPatchVectorField,
Foam::atmBoundaryLayerInletEpsilonFvPatchScalarField
TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/atmBoundaryLayerInletVelocity
This boundary condition specifies a velocity inlet profile appropriate
for atmospheric boundary layers (ABL).
See Foam::atmBoundaryLayer for details.
Example of the boundary condition specification:
\verbatim
ground
{
type atmBoundaryLayerInletVelocity;
n (1 0 0);
z (0 0 1);
Uref 10.0;
Zref 20.0;
z0 uniform 0.1;
zGround uniform 0.0;
}
\endverbatim
See also
Foam::atmBoundaryLayer,
Foam::atmBoundaryLayerInletKFvPatchScalarField,
Foam::atmBoundaryLayerInletEpsilonFvPatchScalarField
TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/turbulentMixingLengthDissipationRateInlet
This boundary condition provides a turbulence dissipation, \f$\epsilon\f$
(epsilon) inlet condition based on a specified mixing length. The patch
values are calculated using:
\f[
\epsilon_p = \frac{C_{\mu}^{0.75} k^{1.5}}{L}
\f]
where
\vartable
\epsilon_p | patch epsilon values
C_{\mu} | Model coefficient, set to 0.09
k | turbulence kinetic energy
L | length scale
\endvartable
Usage
\table
Property | Description | Required | Default value
mixingLength | Length scale [m] | yes |
phi | flux field name | no | phi
k | turbulence kinetic energy field name | no | k
\endtable
Example of the boundary condition specification:
\verbatim
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005;
value uniform 200; // placeholder
}
\endverbatim
Note
In the event of reverse flow, a zero-gradient condition is applied
See also
Foam::inletOutletFvPatchField
TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/turbulentMixingLengthFrequencyInlet
This boundary condition provides a turbulence specific dissipation,
\f$\omega\f$ (omega) inlet condition based on a specified mixing length.
The patch values are calculated using:
\f[
\omega_p = \frac{k^{0.5}}{C_{\mu}^{0.25} L}
\f]
where
\vartable
\omega_p | patch omega values
C_{\mu} | Model coefficient, set to 0.09
k | turbulence kinetic energy
L | length scale
\endvartable
Usage
\table
Property | Description | Required | Default value
mixingLength | Length scale [m] | yes |
phi | flux field name | no | phi
k | turbulence kinetic energy field name | no | k
\endtable
Example of the boundary condition specification:
\verbatim
{
type turbulentMixingLengthFrequencyInlet;
mixingLength 0.005;
value uniform 200; // placeholder
}
\endverbatim
Note
In the event of reverse flow, a zero-gradient condition is applied
See also
Foam::inletOutletFvPatchField
compressible/rhoCentralFoam/BCs/mixedFixedValueSlip
A mixed boundary type that blends between fixedValue and slip, as opposed
to the standard mixed condition that blends between fixedValue and
fixedGradient; required to implement maxwellSlipU condition.
compressible/rhoCentralFoam/BCs/rho
Foam::fixedRhoFvPatchScalarField
This boundary condition provides a fixed density inlet condition for
compressible solvers, where the density of calculated using:
\f[
\rho = \psi p
\f]
where
\vartable
p | pressure [Pa]
\rho | density [kg/m3]
\endvartable
Usage
\table
Property | Description | Required | Default value
p | Pressure field name | no | p
psi | Compressibility field name | no | thermo:psi
\endtable
Example of the boundary condition specification:
\verbatim
{
type fixedRho;
}
\endverbatim
compressible/rhoCentralFoam/BCs/T
Smoluchowski temperature jump boundary condition
compressible/rhoCentralFoam/BCs/U
Maxwell slip boundary condition including thermal creep and surface
curvature terms that can be optionally switched off.
incompressible/adjointShapeOptimizationFoam/adjointOutletPressure
incompressible/adjointShapeOptimizationFoam/adjointOutletVelocity
multiphase/compressibleMultiphaseInterFoam/multiphaseMixtureThermo/alphaContactAngle
Contact-angle boundary condition for multi-phase interface-capturing
simulations. Used in conjuction with multiphaseMixture.
multiphase/multiphaseEulerFoam/multiphaseSystem/alphaContactAngle
Contact-angle boundary condition for multi-phase interface-capturing
simulations. Used in conjuction with multiphaseSystem.
multiphase/multiphaseInterFoam/multiphaseMixture/alphaContactAngle
Contact-angle boundary condition for multi-phase interface-capturing
simulations. Used in conjuction with multiphaseMixture.
multiphase/reactingEulerFoam/reactingMultiphaseEulerFoam/multiphaseSystem/alphaContactAngle
Contact-angle boundary condition for multi-phase interface-capturing
simulations. Used in conjuction with multiphaseSystem.
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/derivedFvPatchFields/alphatFixedDmdtWallBoilingWallFunction
A simple alphatPhaseChangeJayatillekeWallFunctionFvPatchScalarField with
a fixed volumetric phase-change mass flux.
See also
Foam::compressible::
alphatPhaseChangeJayatillekeWallFunctionFvPatchScalarField
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/derivedFvPatchFields/alphatPhaseChangeJayatillekeWallFunction
This boundary condition provides a thermal wall function for turbulent
thermal diffusivity (usually\c alphat) based on the Jayatilleke model for
the Eulerian multiphase solvers.
Usage
\table
Property | Description | Required | Default value
Prt | Turbulent Prandtl number | no | 0.85
Cmu | Model coefficient | no | 0.09
kappa | von Karman constant | no | 0.41
E | Model coefficient | no | 9.8
\endtable
Example of the boundary condition specification:
\verbatim
{
type alphatPhaseChangeJayatillekeWallFunction;
Prt 0.85;
kappa 0.41;
E 9.8;
value uniform 0; // optional value entry
}
\endverbatim
See also
Foam::compressible::alphatPhaseChangeWallFunctionFvPatchScalarField
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/derivedFvPatchFields/alphatWallBoilingWallFunction
A thermal wall function for simulation of subcooled nucleate wall boiling.
Implements a version of the well-known RPI wall boiling model
(Kurul & Podowski, 1991). The model implementation is similar to the model
described by Peltola & Pattikangas (2012).
References:
\verbatim
"On the modeling of multidimensional effects in boiling channels"
Kurul, N., Podowski, M.Z.,
ANS Proceedings, National Heat Transfer Conference,
Minneapolis, Minnesota, USA, July 28-31, 1991,
ISBN: 0-89448-162-1, pp. 30-40
\endverbatim
\verbatim
"Development and validation of a boiling model for OpenFOAM
multiphase solver"
Peltola, J., Pattikangas, T.J.H.,
CFD4NRS-4 Conference Proceedings, paper 59,
Daejeon, Korea, September 10-12 2012
\endverbatim
See also
Foam::fixedValueFvPatchField
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/derivedFvPatchFields/copiedFixedValue
Copies the boundary values from a user specified field.
See also
Foam::fixedValueFvPatchField
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/derivedFvPatchFields/fixedMultiPhaseHeatFlux
Calculates a wall temperature that produces the specified overall wall heat
flux across all the phases in an Eulerian multi-phase simulation.
Intended to be used with copiedFixedValue to ensure that phase wall
temperature are consistent:
- Set 'fixedMultiPhaseHeatFlux' boundary for one of the phases
- Use 'copiedFixedValue' for all the other phases.
See also
Foam::fixedValueFvPatchField
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/kineticTheoryModels/derivedFvPatchFields/JohnsonJacksonParticleSlip
Partial slip boundary condition for the particulate velocity.
References:
\verbatim
"Multifluid Eulerian modeling of dense gas?solids fluidized bed
hydrodynamics: Influence of the dissipation parameters"
Reuge, N.,
Chemical Engineering Science
Volume 63, Issue 22, November 2008, pp. 5540-5551
\endverbatim
\verbatim
"Frictional-collisional constitutive relations for granular materials,
with application to plane shearing"
Johnson, P.C., and Jackson, R.,
Journal of Fluid Mechanics
Volume 176, March 1987, pp. 67-93
\endverbatim
multiphase/reactingEulerFoam/reactingTwoPhaseEulerFoam/twoPhaseCompressibleTurbulenceModels/kineticTheoryModels/derivedFvPatchFields/JohnsonJacksonParticleTheta
Robin condition for the particulate granular temperature.
References:
\verbatim
"Multifluid Eulerian modeling of dense gas?solids fluidized bed
hydrodynamics: Influence of the dissipation parameters"
Reuge, N.,
Chemical Engineering Science
Volume 63, Issue 22, November 2008, pp. 5540-5551
\endverbatim
\verbatim
"Frictional-collisional constitutive relations for granular materials,
with application to plane shearing"
Johnson, P.C., and Jackson, R.,
Journal of Fluid Mechanics
Volume 176, March 1987, pp. 67-93
\endverbatim
multiphase/twoPhaseEulerFoam/phaseCompressibleTurbulenceModels/kineticTheoryModels/derivedFvPatchFields/JohnsonJacksonParticleSlip
Partial slip boundary condition for the particulate velocity.
References:
\verbatim
"Multifluid Eulerian modeling of dense gas?solids fluidized bed
hydrodynamics: Influence of the dissipation parameters"
Reuge, N.,
Chemical Engineering Science
Volume 63, Issue 22, November 2008, pp. 5540-5551
\endverbatim
\verbatim
"Frictional-collisional constitutive relations for granular materials,
with application to plane shearing"
Johnson, P.C., and Jackson, R.,
Journal of Fluid Mechanics
Volume 176, March 1987, pp. 67-93
\endverbatim
multiphase/twoPhaseEulerFoam/phaseCompressibleTurbulenceModels/kineticTheoryModels/derivedFvPatchFields/JohnsonJacksonParticleTheta
Robin condition for the particulate granular temperature.
References:
\verbatim
"Multifluid Eulerian modeling of dense gas?solids fluidized bed
hydrodynamics: Influence of the dissipation parameters"
Reuge, N.,
Chemical Engineering Science
Volume 63, Issue 22, November 2008, pp. 5540-5551
\endverbatim
\verbatim
"Frictional-collisional constitutive relations for granular materials,
with application to plane shearing"
Johnson, P.C., and Jackson, R.,
Journal of Fluid Mechanics
Volume 176, March 1987, pp. 67-93
\endverbatim
stressAnalysis/solidDisplacementFoam/tractionDisplacement
Fixed traction boundary condition for the standard linear elastic, fixed
coefficient displacement equation.
stressAnalysis/solidEquilibriumDisplacementFoam/tractionDisplacementCorrection
Total 191
|